Introduction

FreeCAD is a parametric 3D computer-aided design / modeling tool. It contains different segments of functionality, referred to as workbenches. Each workbench targets a different aspect of the overall design workflow (e.g., sketching, turning sketches into 3D objects, and assembling 3D objects together).

The following subsections give a basic overview and usage reference for the subset of workbenches related to 3D printing.

User Interface Layout

Regardless of which workbench you're in, FreeCAD's UI will likely have the sections highlighted in the screenshot above. Almost everything in the toolbar can also be accessed via the main menu and triggered via a keyboard shortcut.

Viewport

• (6) Viewport: The space in which work in performed. The viewport typically renders and allows control of geometry (e.g., 3D primitives, 2D sketches, and technical drawings). For some workbenches, the viewport displays something different than geometry (e.g., spreadsheet).

• (11) Navigation cube: When working in 3D, there will be a navigation cube (located in the viewport's top right in the example) that reduces the burden rotating and reorienting viewing angles, as well as changing perspectives. Clicking the various faces of the cube as well as the surrounding icons reorient the camera and change perspective.

• (12) Axis orientation: When working in 3D, the basis axes will be displayed from the current camera's orientation (located in the viewport's button right in the example).

• (10) 3D viewport boundaries / spatial unit selection: When the viewport is viewing geometry, this dropdown can be used to change the units of measurement used (e.g., metric to imperial). It also displays the bounds of the viewport in those units of measurement.

• (9) 3D viewport mouse controls: When working in 3D, the mouse controls can be changed to different presets using this dropdown (e.g., Blender style mouse controls vs mouse controls optimized for a trackpad).

  Hovering over the dropdown displays how mouse controls for the currently selected configuration (e.g., what right-click does).

• (3) 3D viewport helpers: When working in 3D, these toolbar buttons provide quick tools to adjust and reorient the view. From left-to-right, ...

  • zoom viewport in to all geometry.
  • zoom viewport in to selected geometry.
  • drop-down to reorient viewing angle and change perspective (e.g., orthographic vs perspective), providing similar to the navigation cube in the viewport.
  • reorient camera to point facing the selection (e.g., point towards face using face's normal vector).
  • drop-down to change how viewport shades models.
  • drop-down to filter mouse selections to only target specific types of 3D entity (e.g., point vs edge vs face)
  • drop-down providing access to various selection helpers (e.g., change how panels synchronize when something's selected)
  • launch measurement tool (e.g., measure area of selected faces or measure distance between two points).

Document hierarchy / operations

• (4) Model pane: List of open documents, as well as the hierarchy of each open document. In the example, the document Test3 has a part design body with a sketch in it.

• (5) Properties pane: For the selected items, this pane lists the properties for those items. If the item is selected within a 3D viewport, the Data tab below shows the physical properties (e.g., what it is) while the View tab below shows the visual properties (e.g., how its rendered).

  Note that properties are not limited to what's selected in the viewport. When an item in the model pane is selected, it has its properties show up.

• (7) Workspace tabs: Tabs to switch between workspaces.

Basic operations

• (1) Basic commands: These toolbar buttons give quick access to common operations. From left-to-right, ...

  • new document.
  • open document.
  • save document.
  • undo drop-down, which lists and allows going back to previous state.
  • redo drop-down, which lists and allows going forward to subsequent state after an undo.
  • recompute, which recomputes calculations for the current selection or the active document if nothing is selected within it.

• (2) Workbench switcher: Drop-down that switches between workbenches.

• (8) Diagnostic messages: Pop-out that displays log messages. The number displayed is the number of unread diagnostics messages.

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Spreadsheet Workbench

FreeCAD has a built-in spreadsheet and expression engine, accessible through the spreadsheet workbench. A spreadsheet is typically used to store parameters and run formulas, which then go on to be used as the parameters of geometry and other properties of an object. It can also go the other way, pulling data out of a model into a spreadsheet.

User Interface

Basic operations

• (1) Basic commands: These toolbar buttons give quick access to common operations. From left-to-right, ...

  • new spreadsheet.
  • import CSV as new spreadsheet.
  • export spreadsheet to CSV.

Viewport

• (10) Spreadsheet: A matrix of cells, identified by column letter and row number (e.g., C3).

  Type while a cell is selected to set that cell's contents. Right click on a row/column to add or remove rows/columns.

• (9) Cell alias textfield: This field shows and sets the alias for the selected cell, similar to pressing the cell alias button in the toolbar. When referencing a cell, the alias can be used as a friendly name.

• (8) Cell content: This field shows and sets the content of the cell, which may be a formula or a literal.

• (7) Zoom slider: This slider and accompanying drop-down are used to zoom in / out of the spreadsheet.

Cell operations and properties

• (2) Cell merge/split: These toolbar buttons merge and split cells. From left-to-right, ...

  • merge selected cells into a single cell.
  • split a merged cell back out to its original individual cells.

• (3) Text alignment: These toolbar buttons align text in a cell. From left-to-right, ...

  • align left.
  • align horizontal center.
  • align right.
  • align top.
  • align vertical center.
  • align bottom.

• (4) Text style: These toolbar buttons stylize the text in a cell. From left-to-right, ...

  • bold.
  • italic.
  • underline.

• (6) Cell colors: These toolbar buttons set the colors within a cell. From left-to-right, ...

  • text color.
  • background color.

• (5) Cell alias button: This toolbar option launches a dialog to set an alias for the selected cell. When referencing a cell, the alias can be used as a friendly name.

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Cell Types

A cell's contents may be ...

• a numeric literal: Identified when the cell contains nothing but a fractional
• a text literal: Identified by an apostrophe as the first character.
• an expression (formula): Identified by an equal sign as the first character.

As shown in the example above, formulas are unit-aware (e.g., a formula can add two angles together or two distances together). The cell displays the results in the user's desired unit system (e.g., imperial vs metric).

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Expressions

In addition to being set to literals, spreadsheet cells and other properties may also be set to expressions. An expression executes some piece of logic using basic operators, functions, constants, conditionals, and references to other properties (e.g., other cells or data within a model). Operators and functions are unit-aware, requiring a valid combinations of units if supplied. For example, 2mm + 4mm is valid while 2mm + 4 is not. This also applies to references to properties that have units (e.g., Pad001.Length + 1 isn't valid because it adds a pure number to a property containing a length - it requires Pad001.Length + 1mm).

Units

Numbers in an expression may optional have a unit. The following tables contain the unit designations recognized by FreeCAD when inserting a unit (e.g., 5 mm). The following tables were pulled directly from source.

Angle

Length

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Property Access

An expression can reference properties of other objects by referencing the path hierarchy. For example, if there's a diameter named (diameter constraint) lower_initial_diam within a sketch ...

• with the label my_sketch, it's accessible within the spreadsheet as =<<!!my_sketch!!>>.!!Constraints!!.lower_initial_diam.
• with the ID Sketch, it's accessible within the spreadsheet as =!!Sketch!!.!!Constraints!!.lower_initial_diam.

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Index Access

To reference an item in a list or tuple, use the [] operator. For example, !!Sketch!!.!!Constraints!![0] will pull the first constraint within the sketch object.

To reference an enumeration option's text, use the [] operator in addition to referencing the enumeration option itself. For example, Pad.Type.Enum[Pad.Type] will pull out the text for Pad.Type, while Pad.Type itself will only return it's index within the enumeration.

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Conditionals

Conditional expressions use C++ style ternary operator syntax: condition ? resultTrue : resultFalse. The condition is defined as an expression that evaluates to either 0 (false) or non-zero (true).

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Operators

Table pulled directly from source.

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Constants

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Functions

FreeCAD expressions support several built-in functions. The following sections each contain a subset of useful functions pulled directly from the source documentation.

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Trigonometry

Table pulled directly from source.

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Rounding

Table pulled directly from source.

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Boolean Logic

Table pulled directly from source.

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Statistics Operations

Table pulled directly from source.

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Object Creation

Table pulled directly from source.

matrix(
  a11; a12; a13; a14;
  a21; a22; a23; a24;
  a31; a32; a33; a34;
  a41; a42; a43; a44
)

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String Operations

Strings can also be created via string interpolation using the old Python % syntax for string formatting. For example, <<Cube length is %s and width is %s>> % tuple(Box.Length; Box.Width).

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Vector Operations

Matrix Operations

Rotation and Placement can each be represented by a Matrix. The following functions all take in a Matrix, Rotation, or Placement as their first parameter denoted in the table below by m. The type of the returned object is the same as the object supplied in the first argument except when using mtranslate on a Rotation, in which case a Placement will be returned.

Sketcher Workbench

Sketcher workbench allows creating 2D sketches. These 2D sketches typically go on to by used by other workbenches (e.g., they define the outline of some 3D feature in the creation of models via the part design workbench).

Sketcher workbench has the following core primitives:

• Element: 2D geometric primitive (e.g., point, line, arc, and spline)
• Constraint: Definition of an element's measurement, either directly (e.g., 5mm radius for an arc) or as a relationship (e.g., line 1's slope must be perpendicular to line 2's slope).

In the screenshot below, the red geometry are visualizations of constraints (e.g., angle and radius), while the white lines are the geometric primitives those red lines apply to (e.g., arc).

There are different element types (e.g., construction geometry, projection geometry) and different constraint types (e.g., reference constraints, driving constraints). These are documented in the subsections below.

User Interface

The Sketcher workbench has two modes: Editing a sketch or viewing a sketch. The toolbar buttons change depending on the mode. The UI layout shown in the screenshot above is when editing a sketch, which is the mode that users will spend most of their time in.

General Commands

• (1) General commands: These toolbar buttons give quick access to common operations. When not editing a sketch, the general commands are as follows:

  

  From left-to-right, ...

  • new sketch: Creates a new sketch object in the model pane.
  • edit sketch: Enters the currently select sketch object in the model pane.
  • attach sketch: Attach sketch to an piece of 3D geometry (e.g., face on a model).
  • reorient sketch: Attach sketch to an origin plane (e.g., XY plane).
  • validate sketch: Opens a pane to validate different aspects of the sketch (e.g., invalid constraints).
  • merge sketches: Merge the sketches selected in the model pane.
  • mirror sketch: Mirror the sketch selected in the model pane.

  When editing a sketch, the general commands are as follows:

  

  From left-to-right, ...

  • leave sketch: Stop editing sketch.
  • align view to sketch: Reorients camera such that it faces towards the sketch.
  • toggle section view: Temporarily cut through and hide geometry that occludes a sketch (e.g., when the camera is aligned to the sketch, it may be occluded by currently visible 3D objects).

• (13) Leave sketch.

Elements and Constraints

• (3) Construction geometry toggle.

• (2) Create elements: These toolbar buttons give quick access to create elements. From left-to-right, ...

  • create point.
  • create polyline.
  • create line.
  • create arcs of varying types and parameterizations (e.g., circular arc defined via 3 points, and circular arc defined via radius and angle, and elliptical arc).
  • create circle / ellipse using varying parameterizations (e.g., defined via 3 points, and defined via radius and angle)
  • create rectangles of varying types and parameterizations (e.g., rectangle defined via center and dimensions, e.g., rectangle define via top-left and bottom-right, and rounded rectangle).
  • create polygon with varying number of sides.
  • create slot of varying types.
  • create b-spline of varying types and parameterizations.

• (5) Constraints toggle: These toolbar buttons disable constraints or keep them enabled but render them unenforced (referred to as reference constraints).

• (4) Create constraints: These toolbar buttons give quick access to create constraints. From left-to-right, ...

  • create dimensional constraints of varying types (e.g., distance, radius, and angle)
  • create coincident constraint.
  • create parallel to basis axis constraint (e.g., force line to be horizontal or vertical).
  • create parallel constraint (e.g., lines 1 and 2 must be parallel).
  • create perpendicular constraint (e.g., lines 1 and 2 must be perpendicular).
  • create tangent constraint (e.g., line and endpoint of arc must be tangent).
  • create distance equality constraint (e.g., line 1 and 2 must be the same distance).
  • create symmetry constraint (e.g., points 1 and 2 must be symmetrical across line 1).
  • create block constraint.

• (7) Selection helpers: These toolbar buttons give quick access to select elements / constraints associated with the current selection. From left-to-right, ...

  • select constraints associated with selection.
  • select elements associated with selection.

• (8) Arc circular helper toggle: Toggles the visibility of the underlying circle / ellipse for circular arcs.

• (10) Internal geometry toggle: Toggles the visibility of the internal geometry for certain element types (e.g., ellipse arc).

• (11) Switch virtual space.

B-Splines

• (6) B-spline tools: These toolbar buttons give quick access to b-spline helpers and tools. From left-to-right, ...

  • geometry to b-spline.
  • increase b-spline degree.
  • decrease b-spline degree.
  • increase knot multiplicity.
  • decrease knot multiplicity.
  • insert knot.
  • join b-spline curves.

• (9) B-spline informational toggles: These toolbar buttons give quick access to toggle on/off information displayed for b-splines. From left-to-right, ...

  • b-spline degree visibility toggle.
  • b-spline control polygon visibility toggle.
  • b-spline curvature comb visibility toggle.
  • b-spline knot multiplicity visibility toggle.
  • b-splint control point weight visibility toggle.

Tools

• (12) Tools: These toolbar buttons give quick access to various sketching tools. From left-to-right, ...

  • fillet / chamfer.
  • trim, split, or extend edges.
  • project from external geometry (e.g., pull in an edge from an external model into the sketch) or project intersected external geometry (e.g., pull in an edge from a model face that intersects the sketch plane).

Panels

• (13) Constraints pane: This pane lists, allows selection, and allows configuration of constraints, mirroring whatever is selected in the viewport.

• (14) Elements pane: This pane lists, allows selection, and allows configuration of elements, mirroring whatever is selected in the viewport.

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Sketching

Sketching involves creating elements, constraining them, and deleting them. The sketch below is a non-trivial set of elements chained together using constraints.

The subsections below document these basic concepts.

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Creation

To create an element, select the element from the toolbar (or the main menu, or use the element's shortcut key) and click on the viewport multiple times. For most elements, on the first click the viewport should show that the item is being created, and the movement of the mouse button and subsequent clicks further constructs the element. For example, to add a line, select the line in the toolbar, click in the viewport, and slightly move the mouse. The line's preview will display.

A subsequent click will be complete adding the line.

In the preview, there are two textboxes, one that specifies a distance and one that specifies an angle. These are referred to as On-View-Parameters, and they're available for certain elements, When in preview, pressing Tab will cycle into these textboxes, where a value may be entered followed by pressing Enter. Using them adds constraints to line. For example, if used for the line above, a constraint is added for the line's length and another constraint is added for the line's angle from the horizontal axis.

Alternatively, an element can have constraints added to it by selecting the relevant portions of an element and clicking an applicable constraint. For example, the line can have the exact same constraints applied by ...

• selecting the line, then selecting distance dimension constraint in the toolbar.
• selecting the line and the horizontal access, then selecting the angle dimension constraint in the toolbar.

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Continue Mode

Continue mode allows element / constraint creation to continue after an element / constraint is created, allowing multiple such elements / constraints to be created many times over. The creation tool remains active until the user hits Esc or selects some other tool from the toolbar. For example, after selecting the line element from the toolbar and creating a line on the sketch, more lines can be created on the sketch without having to click the line element again in the toolbar.

Continue mode can be turned off in preferences (on by default).

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On-View-Parameters

For certain element creation tools, On-View-Parameters allows explicitly adding constraints during the creation process by presenting input fields alongside the element's preview. For example, dropping a line will show a textbox for length constraint and a textbox for angle constraint. Pressing tab cycles through these textboxes, while pressing enter adds the constraints.

Continue mode can be turned off and configured in preferences (on by default).

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Auto Constraints

When creating an element, if the placement of some part of that element ends on an existing element, an auto constraint may be applied. An auto constraint is a constraint that's automatically added by virtue of how the elements end up together. For example, if the end of a line ends up on the start of a line, auto constraint will add a constraint known as coincident constraint which bounds those two points together.

When an auto constraint is to be applied, the icon of the constraint is shown on the lower right of the icon of the element being created.

Auto constraints is enabled/disabled per sketch, not globally. To change, update in the constraints pane or the sketch's view Autoconstraints property.

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Selection

Elements and constraints can be selected in any of the following ways:

• Single selection: Left-clicking an element or constraint toggles whether its selected.

  Previously selected elements are not discarded on single select. While it isn't necessary to hold Ctrl while selecting multiple elements, it is beneficial in that a mis-click into empty space won't deselect everything.

• Box selection: Left-clicking an empty area and dragging draws a selection rectangle, selecting elements within the rectangle (not constraints, only selections). Depending on the direction of the drag, the selection behavior changes. If the box dragging is from ...

  • left to right, elements that lie completely inside the rectangle are selected.
  • right to left, elements that touch or cross the rectangle are selected.

  Previously selected elements are not discarded on box select.

• Connection selection: Double-clicking an edge selects all edges directly and indirectly connected to it via endpoints. Endpoints only need to have the same coordinates (no need endpoints to be connected via constraints - e.g.,coincident constraints).

  Previously selected elements are not discarded on connection select.

• Element / Constraints pane: Constraints and the individual sub-elements of each element (e.g., a line elements's endpoint and actual line) are selectable via the constraints pane and elements pane, respectively. The elements pane lists the individual elements as well as the sub-elements for those elements, which can be individually clicked (e.g., select 2-Line's first endpoint).

  

  Previously selected elements are discarded on connection select.

• Select all: To select everything within a sketch, use Ctrl+A or navigate to Edit → Select All.

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Deletion

To delete an element or constraint, select it and hit the Delete key. If an element is deleted, its related constraints are automatically deleted as well, even if they were left unselected when the Delete key was hit.

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Constraint Expressions

Constraints can be named by either ...

• right-clicking on them in the Constraints pane and selecting Rename (shortcut key F2).
• double-clicking the constraint in the viewport and assigning a name, but this only works if the constraint accepts a value.

Constraints can also reference and calculate their values via expressions. The formula button (inside the value textbox, to its right) opens an Expression Editor window that allows entering an expression instead of a constant, similar to inserting a formula in a cell for a spreadsheet.

The expression can access data in the sketch (e.g., other constraints) as well as outside the sketch (e.g., alias in a spreadsheet or field in a VarSet). In the example, the constraint is copying the value of another constraint and multiplying it by 2.

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Projection Geometry

An element is deemed projection geometry if that element was pulled in from a 3D object visible from the sketch. Projection geometry is linked to the 3D object it came from.

To project, select the External Projection toolbar button (keyboard shortcut G, X) and select until the all desired elements have been projected (Esc or select another tool to exit). In some cases, it may be difficult to select the desired external geometry (e.g., it may be on the opposite side of the object, hidden from view). Recall that the camera can be rotated while sketching. If rotated, the camera's rotation can be brought back inline with the sketch by clicking the Align View to Sketch toolbar button (keyboard shortcut Q, P): .

To project intersections with the sketching plane, select the External Intersection toolbar button (keyboard shortcut G, I) and select until all desired elements have been projected (Esc or select another tool to exist). In most cases, it's difficult to select the desired intersections because they're likely blocked from view. Recall that the Toggle Section View toolbar button (keyboard shortcut Q, S) will temporarily cut from view anything that extends past the sketch plane towards the camera: .

The color and line style changes based on the type of projected element and the state of the overall sketch. The screenshot below shows the default colors used by FreeCAD for the various types and states.

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Construction Geometry

An element is deemed as construction geometry if it isn't exposed to consumers of the sketch (it's internal to the sketch, hidden once the sketch is closed). Construction geometry is used within the sketch to assist in constraining other geometry.

Construction geometry comes in different forms:

• Construction geometry: A normal element in the sketch is construction geometry.

  

• Projected geometry that's also construction geometry: A projected element in the sketch is construction geometry.

  

• Internal alignment geometry: Construction geometry added by and tied to a complex element, used to control that element (e.g., ellipse control arms).

  

To toggle one or more elements to / from construction geometry, select the elements and click the toggle construction geometry button (keyboard shortcut G,N):

To toggle element creation from / to construction geometry, ensure nothing is selected and click te toggle construction geometry button. Toolbar buttons to create elements will change color to indicate that elements being created are construction geometry.

The color and line style changes based on the type of construction element and the state of the overall sketch. The screenshot below shows the default colors used by FreeCAD for the various types and states.

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Degrees of Freedom

If an element ...

• isn't constrained to the point where it's locked into a specific parameterization (e.g., location, rotation, angle, and whatever other parameters it may have), it's said to have n degrees of freedom, where n >= 1.
• is constrained to the point where it's locked into a specific parameterization, it's said to be fully constrained (0 degrees of freedom).

A degree of freedom is a parameterization that hasn't been set. For example, ...

• a point has 2 degrees of freedom:

  1. X position.
  2. Y position.

  The example below fully constrains a point by setting its position in relation to the origin of the sketch.

  

• a line has 4 degrees of freedom:

  1. Start point's X position.
  2. Start point's Y position.
  3. End point's X position.
  4. End point's Y position.

  The example below fully constrains a line by setting the position of its first point to the origin, and then giving it and angle and a length. The position of the second point is derived from the combination of angle and length.

  

• an arc has 5 degrees of freedom:

  1. Center point's X position.
  2. Center point's Y position.
  3. Radius/diameter of arc's underlying circle.
  4. Angle between the two points comprising the arc.
  5. What segment of the underlying circle the arc sits on.

  The example below fully constrains an arc by setting its center point to the origin of the sketch, setting the radius to 14mm, setting the angle of the arc to 45 degrees, and positioning the arc on the underlying circle by stating that the lower point sits 7mm above the X axis.

  

The overall constraint state for all elements in the sketch is shown in the Sketch Edit pane.

• Under-constrained / Fully constrained: When there's 1 or more degrees of freedom, the Sketch Edit pane will report that the sketch is under-constrained. When there's exactly 0 degrees of freedom, the Sketch Edit pane will report that the sketch is fully constrained. In the example below, the two lines each have a point with a coincident constraint to the origin while the other endpoint is unconstrained (4 degrees of freedom). Clicking the degrees of freedom text in the Sketch Edit pane will will select the two unconstrained endpoints.

  

• Redundant constraints / Partially redundant: If a sketch has constraints that deduce to the same thing, the Sketch Edit pane will report that the sketch has redundant constraints. In the example below, the line's start point has a coincident constraint to the origin and ...

  • the end point has a horizontal distance constraint and vertical distance constraint, both set to 1mm.
  • the line itself has a an angle constraint set to 45 degrees from the X axis.

  This reports a redundant constraint because the end point of (1mm, 1mm) implies a 45 degree angle from the X axis. Clicking the redundant constraints text in the Sketch Edit pane selects the redundant constraints.

  

• Over-constrained: If a sketch has conflicting constraints (they both can't be satisfied because they're opposed to each other), the Sketch Edit pane will report that the sketch has over-constrained. In the example below, the triangle in this sketch is constrained to be an equilateral triangle, but it also has a coincident constraint that says two of the triangle's vertices should be at the same point, making it an impossible to satisfy all constraints. Clicking the over-constrained text in the Sketch Edit pane selects the conflicting constraints.

  

  Typically, once a conflicting constraint is added, the number of conflicting constraints reported becomes much more than 2. That's usually because the 1 added constraint goes is invalid against many existing constraints. The Sketch Edit pane doesn't group conflicting constraints together (e.g., 1,3,5 are valid together vs 2,4 are valid together, but all together they conflict) or give any reasoning as to why the constraints conflict (e.g., deduced angle is 30 degrees but angle constraint is attempting to set to 45 degrees).

It is important that a completed sketch always be fully constrained, otherwise the solver (software responsible for applying constraints) may shift and reorient the elements on that sketch based on the what is and isn't constrained. Even if a sketch is fully constrained, it may still be subject to sketch flipping, a phenomenon where the sketch changes because even when fully constrained there is more than 1 possible outcome for the constraints. In the example below, both arcs have the exact same constraints (both fully constrained), but there are two possible solutions.

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Sketch Flipping

Even if a sketch is fully constrained, it may still be subject to sketch flipping, a phenomenon where the sketch reshapes because even when fully constrained there is more than 1 possible outcome for the constraints.

• Example 1

  In the example below, both arcs have the exact same constraints (both fully constrained), but there are two possible solutions.

  

  Sketch flipping happens because, in certain cases, directionality may not exist. There's no constraint that ties the arc as to which side of the X axis it's on.

  This can be fixed by adding a constraint to force directionality. For example, adding a horizontal constraint between the end of the arc and the origin adds directionality. A horizontal constraint / vertical constraint is signed, meaning that a value of 12mm goes in one direction while -12mm goes in the opposite direction.

  

• Example 2

  In the example below, both shapes have the exact same constraints (both fully constrained) except that the second version is 50mm away from the Y axis instead of 16mm. Note that the sketch changed shape even though all other constraints are equivalent.

  

  As with the previous example, there is a lack of directionality that causes sketch flipping. The top horizontal line has a distance constraint of 10mm, but there's nothing constraining the order of the points (which of its two points is closer to the Y axis). The solver is free to swap the points as it sees fit, so long as the distance is still 10mm.

  Again, this can be fixed by adding a constraint to force directionality. For example, instead of using a distance constraint of 10mm, using a horizontal constraint of 10mm will. A horizontal constraint with a value of 10mm will fix the sketch into one orientation, while -10mm will fix it into the other orientation.

  

• Example 3

  The example below is similar to the previous example, except more complex. There's double flipping occurring:

  1. The box and triangle are flipping across the symmetry line
  2. The box has flipped such that the vertical line closer to the symmetry line has become the one farther from the symmetry line.

  

  Again, this can be fixed by adding one or more constraints to force directionality:

  • Add a horizontal constraint to the box to ensure its points don't flip.
  • Add a horizontal constraint between the symmetry line's point and either a point on the box or a point on the triangle, to ensure they stay on the correct side of the symmetry line.

  

To prevent flipping, it's important to anchor the sketch using constraints that support directionality. In general ...

• horizontal constraints are signed, so they can specify directionality.
• vertical constraints are signed, so they can specify directionality.
• angle constraints are signed, so they can specify directionality, but that only works if the angle is anchored to something fixed (e.g., angle from x-axis and not the angle for an arc).
• block constraints force an exact position, similar to adding a horizontal constraint and vertical constraint against the origin.

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Elements

An element is a 2D geometric primitive (e.g., point, line, arc, and spline). The element itself defines a primitive, while the parameterization of the primitive are defined by constraints applied to the element (constraints are discussed in later sections).

The subsections below detail the various elements available.

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Point

To create a point, use toolbar button 1 (keyboard shortcut G,Y) and click within the 3D viewport to place the point.

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Line

To create a line, use toolbar button 3 (keyboard shortcut G,L). Once the tool is active, select the mode in which the line should be created (cycle keyboard shortcut M). The mode defines the constraints presented by On-View-Parameters when the line is being created:

• Point, length, angle
• Point, width, height
• 2 points (no constraints presented)

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click again to place the second point.

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Rectangle

To create a rectangle, use toolbar button 6 to present a drop-down and either select ...

• Rectangle (keyboard shortcut G,R)
• Centered Rectangle (keyboard shortcut G,V)
• Rounded Rectangle (keyboard shortcut G,O)

The selection activates the tool with specific Rectangle Parameters preset. Those parameters can continue to be set once the tool is active:

• Mode: The mode in which the rectangle should be created (cycle keyboard shortcut M). Mode defines the constraints presented by On-View-Parameters when the rectangle is being created.
• Rounded corners: Whether the rectangle should have rounded corners (keyboard shortcut U). Rounded corners defines extra elements and constraints to be presented by On-View-Parameters when the rectangle is being created.
• Frame: Whether the rectangle should be a frame (keyboard shortcut J), as in have an inner and outer border. Frame defines extra elements and constraints to be presented by On-View-Parameters when the rectangle is being created.

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete.

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Polygon

To create a polygon, use toolbar button 7 to present a drop-down and either select ...

• Triangle (keyboard shortcut G,P,3).
• Square (keyboard shortcut G,P,4).
• Pentagon (keyboard shortcut G,P,5).
• Hexagon (keyboard shortcut G,P,6).
• Heptagon (keyboard shortcut G,P,7).
• Octagon (keyboard shortcut G,P,8).
• Polygon (keyboard shortcut G,P,R).

Except for Polygon, the selection activates the tool with specific Polygon Parameters preset. Those parameters can continue to be set once the tool is active:

• Mode: Select the number of sides for the polygon (keyboard shortcut U to increase, keyboard shortcut J to decrease).

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete.

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Circle Ellipse

To create an ellipse or circle, use toolbar button 5 to present a drop-down and either select ...

• Circle from Center (keyboard shortcut G,C).
• Circle from 3 Points (keyboard shortcut G,3,C).
• Ellipse from Center (keyboard shortcut G,E,E).
• Ellipse from 3 Points (keyboard shortcut G,3,E).

Once the tool is active, select the mode in which the line should be created (cycle keyboard shortcut M). The mode defines the constraints presented by On-View-Parameters when the line is being created:

• Center: Create circle/ellipse from a center point.
• 3 rim points / Axis endpoints: Create circle/ellipse from 3 points on the rim.

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete.

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Arc

To create an arc, use toolbar button 4 to present a drop-down and either select ...

• Arc from Center (keyboard shortcut G,A).
• Arc from 3 Points (keyboard shortcut G,3,A).
• Elliptical Arc (keyboard shortcut G,E,A).
• Hyperbolic Arc (keyboard shortcut G,H).
• Parabolic Arc (keyboard shortcut G,J).

Of the options, ...

• for the first two (circular arcs), once the tool is active select the mode in which the line should be created (cycle keyboard shortcut M):

  • Center: Create circle/ellipse from a center point.
  • 3 rim points / Axis endpoints: Create circle/ellipse from 3 points on the rim.

  The only mode that defines constraints presented by On-View-Parameters when being created is Center.

  

• for the remainder, there are no options and On-View-Params aren't enabled.

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete.

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Polyline

A polyline is a helper that chains together lines and arcs into a path. To create a polyline use toolbar button 2 (keyboard shortcut G,M). Then, either select where to drop the first point or click an existing endpoint. Continue clicking to place new segments in a chain, hitting M to cycle through the line and arc options:

• Line connected to the previous segment.
• Line perpendicular to the previous segment.
• Line tangential to the previous segment.
• Arc tangential to the previous segment (hold Ctrl to snap arc to increments of 45 degree relative to the previous segment).
• Arc perpendicular (left) to the previous segment (hold Ctrl to snap arc to increments of 45 degree relative to the previous segment).
• Arc perpendicular (right) to the previous segment (hold Ctrl to snap arc to increments of 45 degree relative to the previous segment).

Click within the 3D viewport to place the element and continue clicking to draw. Hit Esc to end.

There must be a previous segment for M to cycle through line and arc options (there will be if you dropped on an existing endpoint). For the initial segment, the mode is always hardcoded to a line (M won't cycle).

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Slot

To create a slot, use toolbar button 8 to present a drop-down and either select ...

• Slot (keyboard shortcut G,S)
• Arc Slot (keyboard shortcut G,S,S)

Slot and Arc Slot are different tools. When ...

• Slot is activated, there are no parameters.

• Arc Slot is activate, there are parameters:

  • Mode: The mode in which the rectangle should be created (cycle keyboard shortcut M). Mode defines the ends of the arc slot (flat vs round).

  

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete.

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B-Spline

To create a b-spline, use toolbar button 9 to present a drop-down and either select ...

• B-Spline (keyboard shortcut G,B,B).
• Periodic B-Spline (keyboard shortcut G,B,P).
• B-Spline from Knots (keyboard shortcut G,B,I).
• Periodic B-Spline from Knots (keyboard shortcut G,B,O).

The selection activates the tool with specific Rectangle Parameters preset. Those parameters can continue to be set once the tool is active:

• Mode: The mode in which the b-spline should be created (cycle keyboard shortcut M). Mode defines whether the clicks in the 3D viewport are for the b-spline's control points or knots.
• Periodic: Whether the b-spline curve loops seamlessly into itself (keyboard shortcut R).

Click within the 3D viewport to place the element and either fill out the On-View-Parameters or click until placement is complete. Hit Esc to end.

There are various b-spline modifiers / helpers:

• Geometry to B-Spline
• Increase B-Spline Degree
• Decrease B-Spline Degree
• Increase Knot Multiplicity
• Decrease Knot Multiplicity
• Insert Knot
• Join Curves

There are various visual helpers for b-splines that can be enabled / disabled:

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Constraints

A constraint limits the possible values for an element's parameters. For example, a line may have an endpoint constrained onto the X-axis, in which case the position of that endpoint must always have a Y position of 0.

The subsections below detail the various constraints available.

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Distance Dimension

A Distance Dimension constraint sets the distance.

To create a Distance Dimension constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., line and arc, point and a line, point and a point).

Then, use toolbar button 1 to present a drop-down and select Distance Dimension (keyboard shortcut K,D). A pop-up will ask for the length value. Once the constraint has been created, press Esc to exit.

Distance Dimension works on the elements most users expect (e.g., distance between two points, distance of a line). It also works on other elements. For example, Distance Dimension can be applied to point and a line, an arc, two circles / arcs, a line and a circle / arc,

By definition, a distance must be a non-negative value. Imagine two points on a horizontal line A and B. The distance between (A,B) is the same as the distance between (B,A). For example, if A=5 and B=4, ...

• the distance from A to B is abs(5-4)=1
• the distance from B to A is abs(4-5)=1.

Given this, it's important to remember that distance does not encode a direction (e.g., if it did, the abs would go away, meaning the distance from B to A would have been -1 instead of 1). This lack of direction means that the sketcher's solver can decide to flip sketches even if the sketch is fully constrained (unless it's somehow further constrained to define a direction). For example below, the rectangle below has two distance constraints, ...

• one on the vertical side (15mm).
• one on the horizontal side (20mm).

Because distance doesn't encode direction, the sketcher can decide to flip the horizontal edges or the vertical edges at any time. Imagine taking the lower-right corner of this rectangle and using a coincident constraint to tie it to the origin. Because the edges can flip, at any time the lower-right corner can become the upper-right corner, upper-left corner, or lower-left corner.

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Horizontal Dimension

A Horizontal Dimension constraint sets the how far apart two elements are, horizontally. Unlike the Distance Dimension constraint, it allows direction via positive and negative values.

To create a Horizontal Dimension constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points on different lines).

Then, use toolbar button 1 to present a drop-down and select Horizontal Dimension (keyboard shortcut L). A pop-up will ask for the length value. Once the constraint has been created, press Esc to exit.

If the selection is ...

• one point, the constraint will be relative from the origin:

  • Positive value places point to the right of Y axis.
  • Negative value places point to the left of Y axis.

• two points, the constraint will be relative from the first selected point:

  • Positive value places second point to the right of the first point.
  • Negative value places second point to the left of the first point.

• one line, the constraints will be applied as if the line's two points were selected. The line's first dropped point during creating is treated as the first point, and the second dropped point is treated as the second point.

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Vertical Dimension

A Vertical Dimension constraint sets the how far apart two elements are, vertically. Unlike the Distance Dimension constraint, it allows direction via positive and negative values.

To create a Vertical Dimension constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points on different lines).

Then, use toolbar button 1 to present a drop-down and select Vertical Dimension (keyboard shortcut I). A pop-up will ask for the length value. Once the constraint has been created, press Esc to exit.

If the selection is ...

• one point, the constraint will be relative from the origin:

  • Positive value places point to the above of X axis.
  • Negative value places point to the below of X axis.

• two points, the constraint will be relative from the first selected point:

  • Positive value places second point above the first point.
  • Negative value places second point below the first point.

• one line, the constraints will be applied as if the line's two points were selected. The line's first dropped point during creating is treated as the first point, and the second dropped point is treated as the second point.

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Lock Position

Lock Position is not a constraint, but a helper that applies both a Vertical Dimension constraint and a Horizontal Dimension constraint to the selection, effectively locking the selection in place.

To apply Lock Position, select the element, use toolbar button 1 to present a drop-down, and select Lock Position (keyboard shortcut K,L). Once the constraint has been created, press Esc to exit.

If the selection is ...

• one point, the constraints will be relative from the origin.
• two points, the constraints will be relative from the the opposing points.
• one line, the constraints will be applied as if the line's two points were selected.

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Radius Dimension

A Radius Dimension constraint sets the radius of circles, arcs, and B-spline weight circles.

To create a Radius Dimension constraint, select an element (e.g., arc), use toolbar button 1 to present a drop-down, and select Radius Dimension (keyboard shortcut K,R). A pop-up will ask for the radius value. Once the constraint has been created, press Esc to exit.

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Diameter Dimension

A Diameter Dimension constraint sets the diameter of circles, and arcs.

To create a Diameter Dimension constraint, select the element (e.g., circle), use toolbar button 1 to present a drop-down, and select Diameter Dimension (keyboard shortcut K,O). A pop-up will ask for the diameter value. Once the constraint has been created, press Esc to exit.

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Angle Dimension

An Angle Dimension sets the angle between two edges, a line an an axis of the sketch, or the aperture angle of a circular arc.

To create a Angle Dimension constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two lines).

Then, use toolbar button 1 to present a drop-down and select Angle Dimension (keyboard shortcut K,A). A pop-up will ask for the angle value. Once the constraint has been created, press Esc to exit.

If the selection is ...

• one line, the constraint will be the angle relative to the horizontal axis.
• one arc, the constraints will be the angle defining how far the arc's endpoints are from each other.
• two lines, the constraints will be an angle between the two lines, where the center is the intersection point of the lines.
• two lines and a point, the constraints will be an angle between the two lines, where the center is the point.

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Radius-Diameter Dimension

Radius-Diameter Dimension is not a constraint, but a helper that applies either a Radius Dimension constraint or a Diameter Dimension constraint to the selection, depending on the type of element it is.

To apply Radius-Diameter Dimension, select the element (e.g., arc), use toolbar button 1 to present a drop-down, and select Radius-Diameter Dimension (keyboard shortcut K,S). A pop-up will ask for the diameter/radius value. Once the constraint has been created, press Esc to exit.

If the selection is ...

• an arc or b-spline weight circle, the constraints will be a Radius Dimension.
• a circle, the constraint will be a Diameter Dimension.

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Dimension

Dimension is not a constraint, but a helper that allows cycling through most possible constraints for the element selection.

To apply Dimension, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points on different lines).

Then, use toolbar button 1 to present a drop-down and select Dimension (keyboard shortcut D). Continue to hit M until the desired constraint appears and click to apply. A pop-up may appear asking for a value (e.g., angle if the constraint is Angle Dimension constraint). Once the constraint has been created, press Esc to exit.

For example, if the selection is two lines, the possible constraints that can be cycled through may include Angle Dimension and Parallel.

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Coincident

A Coincident constraint sets a point to lie on another point, edge (e.g., line, rim of an arc, rim of a circle, b-spline), or basis axis.

To create a Coincident constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., a point and a line).

Then, use toolbar button 2 (keyboard shortcut C). A pop-up will ask for the angle value. Once the constraint has been created, press Esc to exit.

If the selection is ...

• two points, the constraint will place the points on top of each other.
• a point and an edge, the constraints will place the point along the edge.
• a point and a basis axis, the constraints will place the point along the basis axis.

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Horizontal

A Horizontal constraint sets a pair of points or a line to be horizontal.

To create a Horizontal constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points).

Then, use toolbar button 3 to present a drop-down and select Horizontal (keyboard shortcut H). Once the constraint has been created, press Esc to exit.

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Vertical

A Vertical constraint sets a pair of points or a line to be vertical.

To create a Vertical constraint, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points).

Then, use toolbar button 3 to present a drop-down and select Vertical (keyboard shortcut V). Once the constraint has been created, press Esc to exit.

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Horizontal-Vertical

Horizontal-Vertical is not a constraint, but a helper that applies either a Horizontal constraint or a Vertical constraint to the selection.

To apply Horizontal-Vertical, select either ...

• an element (e.g., line)
• a pair of items, where each item can be either an element or a sub-element (e.g., two points).

Then, use toolbar button 3 to present a drop-down and select Horizontal-Vertical (keyboard shortcut A). Once the constraint has been created, press Esc to exit.

If the selection is ...

• closer to being horizontal, a Horizontal constraint will be applied.
• closer to being horizontal, a Vertical constraint will be applied.

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Parallel

A Parallel constraint sets a pair of lines to be parallel.

To create a Parallel constraint, select the elements (e.g., two lines) and use toolbar button 4 (keyboard shortcut P). Once the constraint has been created, press Esc to exit.

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Perpendicular

A Perpendicular constraint sets a pair of lines to be perpendicular.

To create a Perpendicular constraint, select the elements (e.g., two lines) and use toolbar button 5 (keyboard shortcut N). Once the constraint has been created, press Esc to exit.

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Tangent-Colinear

A Tangent-Colinear constraint sets two edges (e.g., line, rim of an arc, rim of a circle, b-spline), or an edge and an basis axis, to be tangent. The constraint treats edges as if they're unbounded (e.g., lines are virtually extend out to infinity and open curves are virtually extended, for the purpose of tangency).

To create a Tangent-Colinear constraint, select the elements (e.g., two lines) and use toolbar button 6 (keyboard shortcut T). Once the constraint has been created, press Esc to exit.

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Equal Constraint

An Equal constraint sets two edges (e.g., line, rim of an arc, rim of a circle, b-spline) to have the same length.

To create an Equal constraint, select the element (e.g., two lines) and use toolbar button 7 (keyboard shortcut E). Once the constraint has been created, press Esc to exit.

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Symmetric

A Symmetric constraint sets two points to mirror each other symmetrically over a line, a basis axis, or around a point.

To create a Symmetric constraint, select the element or element component (e.g., two lines). Then, use toolbar button 8 (keyboard shortcut S). Once the constraint has been created, press Esc to exit.

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Block

A Block constraint fixes an edge (e.g., line, rim of an arc, rim of a circle, b-spline) in place. It's mainly intended for b-splines, which can be difficult to fully constrain otherwise.

To create a Block constraint, select the element (e.g., line) and use toolbar button 9 (keyboard shortcut K, B). Once the constraint has been created, press Esc to exit.

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Part Design Workbench

Part Design workbench allows building a contiguous 3D object, mostly by transforming 2D sketches into 3D features in a linear chain. For example, a sketch of a square that's 5mm by 5mm can be padded by 5mm to create a cube. Then, a sketch of a circle with a 3.5mm diameter can be placed on a face of that cube and pocketed to create a cylindrical hole through that cube.

Features are built out using a non-destructive workflow. That means, as features build on top of other features, it's possible to modify earlier features and have the change cascade down to later features. For example, with cylinder-through-box example above, it's possible to go up and change box's dimensions and fillet its corners. The cylinder cut-out feature will still apply.

The core components of the Part Design workbench are bodies and sketches. A body is a model built mostly by transforming 2D sketches into 3D features.

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User Interface

Body

• (1) Create new body.

Sketch

• (2) Sketch operations: These toolbar buttons give quick access to sketch functionality. A body can contain multiple sketches, where those sketches are attached on to a plane or an existing face of the model. Those sketches are selectable in the Model pane's tree, and each acts (in whole or partially) as the base for a 3D feature (e.g., pad sketch into 3D).

  From left-to-right, ...

  • drop-down to either ...
    • create a sketch (either on plane or face).
    • attach an existing sketch to a face.
    • edit an existing sketch.
  • validate a sketch.

Helpers

• (3) Helpers: These toolbar buttons provide access to helpful tools. From left-to-right, ...

  • analyze selected geometry for errors.
  • create a sub-shape binder, which pulls in geometry from another body / object by referencing it.
  • clone selected into a new body (linked, not copied).

Modeling Features

• (4) Additive features: These toolbar buttons provide access to sketch-to-3D features that add to an object. From left-to-right, ...

  • create a solid by padding a sketch.
  • create a solid by revolving a sketch around an axis.
  • create a solid by creating transitions between two or more sketches (sketches are cross-sections of the solid).
  • create a solid by sweeping a sketch around a helix.
  • create a primitive solid (e.g., box, cylinder, sphere).

• (5) Subtractive features: These toolbar buttons provide access to sketch-to-3D features that remove from an object. From left-to-right, ...

  • cut-out from a solid by sinking a sketch.
  • cut-out from a solid by cutting fastener holes (sketch must contain one or more circles).
  • cut-out from a solid by revolving a sketch around an axis.
  • cut-out from a solid by creating transitions between two or more sketches (sketches are cross-sections of the solid).
  • cut-out from a solid by sweeping a sketch around a helix
  • cut-out from a solid by cutting out a primitive solid (e.g., box, cylinder, sphere)

• (6) Import bodies and apply a boolean operation (e.g., intersection).

• (7) Dress-up: These toolbar buttons provide access to some basic non-sketch based features. From left-to-right, ...

  • round selected edges / vertexes.
  • chamfer selected edges / vertexes.
  • angle selected face.
  • convert body to a shell, leaving selected faces open.

Transformation Features

• (8) Transformations: These toolbar buttons pattern on or more features. From left-to-right, ...

  • mirror one or more features.
  • create a linear pattern of one or more features.
  • create a polar pattern of one or more features.
  • create a pattern by combining the transformations mentioned above, as well as scale.

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Organization

The core components of the Part Design workbench are bodies, features, and sketches. A body is a contiguous model created by chaining together distinct steps, known as features. Each feature is a distinct and editable step in the building of that body, and it's typically an extension of a sketch into 3D geometry (e.g., a sketch drawn on a face is extruded/padded to create a new addition).

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Body

A body is a single contiguous 3D model, mostly built by extending sketches into 3D geometry in a chain. Each item in the chain is referred to as a feature, which is a distinct and editable step in the building of the model.

The list of features nested under a body comprise a non-destructive workflow. For example, a sketch of a square that's 5mm by 5mm can be padded by 10mm to create a rectangular prism. Then, a sketch of a circle with a 3.5mm diameter can be placed on a face of that prism and pocketed to create a cylindrical hole through that cube.

Create

Use toolbar button 3 to create a body. For certain operations, if there is no body, one is implicitly created when the operation runs (e.g., creating a new sketch from the Part Design workbench).

Clone

Use toolbar button 8 to clone the current body selected in the Model pane into a new body. A clone is linked, not copied. That means changing the original changes the clone.

Local Coordinate System

Each body has its own local coordinate system that features nested within it are relative to. The properties of a body define its position and rotation within its parent container. In most cases, that parent container is a standard part_FC, but a body can also live outside of a standard part_FC.

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Tip

A body's tip_FC is the index its feature chain that defines the current working point and current geometry. For example, consider a body consisting of 5 features (index 0 to 4) but having its tip_FC set to index 2. The feature at index 2 is what defines the body's overall geometry (any feature after index 2 is ignored), and adding a feature will inject that feature as index 3 and move the tip_FC over to it.

By default, a body's tip_FC is set to the last feature in the chain. To move it a different index, use the right-click the feature in the Model pane and select Set Tip

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Base Feature

A base feature is a reference to an existing object that's imported as the first step of a body. A base feature object is always a live reference. Changes to the source object are automatically applied to the body.

A base feature can be added in many ways:

• Select an existing object and create a clone (toolbar button 8).
• Select an existing object and create a new body (toolbar button 3) sometimes creates that body with the object as its base feature.
• Create a new body and select an object for its Base Feature property in the Model pane.

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Subshape Binder

A subshape binder is a reference to an existing object that's imported as a design reference (e.g., it isn't part of the model, but acts more as helper geometry to construct the model). To add a subshape binder, ...

1. ensure the body is active.
2. select the outside geometry.
3. click subshape binder in the toolbar (green blob with 3 dots) to create a subshape binder object in the body.

The subshape binders Bind Mode property defines if it copies the original geometry or just links to it:

• Synchronized: Live reference. Updates when source changes.
• Frozen: Keeps link, but shape is frozen until refreshed/changed.
• Detached: Copy/snapshot. Breaks live dependency, keeps current shape.

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Sketch

Sketches are core to building out a body. As such, the Part Design workbench provides quick access to sketching functionality.

Creation

To create a sketch, use toolbar button 4 and select New Sketch. If the 3D viewport has ...

• a face selected, the sketch will be placed on the face's plane.
• nothing is selected, the 3D viewport will present the standard basis axis planes (e.g., XY plane, XZ plane). Selecting one of those planes will place the sketch will be placed on that plane.

Once created, the sketch will be entered in Edit mode (Sketcher Workbench will activate). Clicking the Leave Sketch button in the toolbar / clicking the Leave button above the Sketch Edit pane will pop out of the sketch and back into Part Design.

Edit

To edit an existing sketch, select the sketch in the Model pane or 3D viewport, then use toolbar button 4 and select Edit Sketch.

Attach

To attach an existing sketch to something else (e.g., another face), select the thing to attach, then use toolbar button 4 and select Attach Sketch. A dialog will pop-up asking for which sketch to attach, then a subsequent dialog will pop-up asking for the method of attachment (should be Plane face most of the time.)

Validate

To validate an existing sketch, select the sketch in the Model pane or 3D viewport, then use toolbar button 5. A Sketch Validation pane should appear wit buttons to test for specific issues.

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3D Feature Validity

For a sketch to be valid for use as a 3D feature (e.g., as a profile that extrudes into a 3D addition or punches into a 3D face), it must conform to several expectations:

• No open contours: A contours must be closed, meaning gaps between endpoints of that contour aren't allowed (no matter how small).

  

• No intersection: A contour must not intersect with other contours or self-intersect.

  

  ⚠️NOTE️️️⚠️

  While it contours can't intersect, one contour is allowed to be wholly contained in the. See further down for more information.

• No shared edges between contours: Two contours must not share an edge.

  

• No T-connections: A contour must not have two edges sharing a common point / point touching an edge.

  

Contours are allowed to be nested (but not intersecting). Nesting alternates between creating voids in the 3D feature.

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Features

The subsections below detail feature types supported by the Part Design workbench. Most features present a Preview pane during creation.

• Show preview overlay: Presents a see-through overlay of what the feature looks like as parameters are being manipulated.
• Show final result: Presents what the feature looks like as parameters are being manipulated.

Creation may also insert gizmos during creation that mirror parameters of whatever is being created. The example below has a arrow gizmo to control the depth parameter.

Pad / Pocket

A pad operation and a pocket operation are effectively the same thing, except that ...

• pad is additive (creates a solid and merges it with existing geometry it collides with).
• pocket is subtractive (creates a solid and cuts out it from existing geometry it collides with).

To pad / pocket, select a sketch and use either toolbar button 9 (pad) or toolbar button 15 (pocket). Once selected, gizmos appear in the 3D viewport and a parameter pane opens.

The Mode parameter defines which directions the sketch is extruded in:

• One sided: Extrude in one direction.
• Two sided: Extrude in one direction as well as the opposite direction, where each direction has its own set of parameters (e.g., each direction has its own length).
• Symmetric: Extrude symmetrically in one direction as well as the opposite direction (e.g., one length applied to both directions).

One sided and Two sided both enable the Reversed parameter, which reverses direction / directions of extrusion.

The Type parameter defines the stopping point of the extrusion:

• Dimension: Manually define extrusion length and taper angle. When selected, multiple gizmos appear in the 3D viewport. The arrow gizmo controls the Length parameter, while the arc gizmo controls the Taper parameter.
• To last: Extrude until the last intersecting face.
• To first: Extrude until the first intersecting face.
• To face: Extrude until a specific face.
• To shape: Extrude until a specific shape, or a face on a specific shape.

The Direction parameter defines the direction of the sketch's extrusion:

• Sketch normal: Normal vector of the sketch.
• Select reference...: Direction of an edge / datum line.
• Custom direction: Manually define a vector.

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Hole

A hole operation cuts out a standardized fastener hole from existing geometry it collides with (e.g., hole for a screw or nail).

To create a hole, create a sketch with one or more circles, arcs, and/or points (other entities are ignored). Then, select the sketch and use toolbar button 16. Once selected, gizmos may appear in the 3D viewport and a parameter pane opens.

The Base profile types parameter defines which sketch element types to make into holes:

• Points, circles and arcs: Position holes at points as well as the centers of circles and arcs.
• Circles and arcs: Position holes the centers of circles and arcs.
• Points: Position holes at points.

The Standard and Size parameters define the thread standard to target. For example setting Standard to ISO metric regular and Size to M2x0.4 sets all holes to have a diameter of 2mm and a thread pitch of 0.4mm between peaks.

The Head type parameters defines what type / standard of screw head to model the hole for:

• Countersink introduces properties Head diameter, Head depth, and Countersink angle.
• Counterbore introduces properties Head diameter and Head depth.
• Counterdrill introduces properties Head diameter, Head depth, and Countersink angle.

The Depth type parameter defines where the hole stops:

• Through all: The hole goes through everything (Depth parameter disabled).
• Dimension: The hole stops at a certain depth.

Below Depth type is a picture that shows the general type of fastener to expect based on the properties chosen (e.g., the type of head, if its got a pointy head). The picture highlights several attributes of the fastener, where those attributes are linked to fields that configure those attributes. For example, in the example screenshot linked to several fields, the ...

• depth of the fastener is defined by Depth (Depth is disabled if Depth type is set to Through all).
• width of the fastener is is defined by Diameter (Diameter is hardcoded if a Standard and Size were set other than None).
• sharpness of the fastener's tip is defined by Drill angle, and Include in depth defines if the tip is additional to the Depth field's value or added on top of it.

The Switch direction parameter reverses the direction of the hole cut-outs.

The Tapered parameter tapers the hole.

The Hole type parameter defines how holes should treat threads:

• Clearance / Passthrough makes the hole big enough for the fastener with threads, such that the fastener goes through the hole and threads into something else (e.g., a nut on the other end). Selecting this enables the field Clearance, which controls how loose / tight the hole should be for the fastener.

  ⚠️NOTE️️️⚠️

  Clearance isn't documented anywhere, but when you change it you can see the hole slightly expand / contract.

• Tap drill makes the hole a big enough for the fastener without the threads, such that the threads can cut into the hole (e.g., imagine making a pilot hole in a block of wood and then putting a screw in that hole). Selecting this enables the Thread subsection:

  • Class: Thread tolerance / fit class for a threaded hole. Available values depend on Standard.
  • Right hand vs Left hand: Whether the threads tighten clockwise (the standard - righty-tighty vs lefty-loosey) or counterclockwise.
  • Thread Depth Type: When the thread stops (e.g., hole may be 10mm but threads may stop at 5mm). A value of Hole depth threads the entire hole, Dimension allows a custom depth, and Tapped (DIN76) eaves a standard unthreaded relief/runout at the bottom.

  ⚠️NOTE️️️⚠️

  It doesn't look like these parameters do anything for this option? They only seem to do something for the Modeled thread option.

• Modeled thread makes the hole include threads, such that the fastener goes in cleanly. Selecting this enables the Thread subsection:

  • Update thread view: Show the threads in the hole as opposed to just storing metadata about the threads.
  • Class: Thread tolerance / fit class for a threaded hole. Available values depend on Standard.
  • Right hand vs Left hand: Whether the threads tighten clockwise (the standard - righty-tighty vs lefty-loosey) or counterclockwise.
  • Thread Depth Type: When the thread stops (e.g., hole may be 10mm but threads may stop at 5mm). A value of Hole depth threads the entire hole, Dimension allows a custom depth, and Tapped (DIN76) eaves a standard unthreaded relief/runout at the bottom.
  • Custom Clearance: Widens the hole by some amount (e.g., compensate for 3D printing inaccuracies and line width).

  ⚠️NOTE️️️⚠️

  Update thread view physically inserts the threads into the model, but this lags / slows FreeCAD incredibly. It may be a good idea to leave this disabled until the very end. I suspect you need this enabled when exporting to STL or else the threads won't show up. Documentation doesn't talk about this at all.

  Class seems to add some small amount of clearance for ISO types when the class is G. For UTS, I didn't see any value add any clearance. Documentation doesn't talk about this at all.

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Revolution / Groove

A revolution operation and a groove operation are effectively the same thing, except that ...

• revolution is additive (creates a solid and merges it with existing geometry it collides with).
• groove is subtractive (creates a solid and cuts out it from existing geometry it collides with).

To revolve / groove, select a sketch and use either toolbar button 10 (revolution) or toolbar button 17 (groove). Once selected, gizmos appear in the 3D viewport and a parameter pane opens.

The Type parameter defines which directions the sketch is extruded in:

• Angle: Extrude in one direction.
• Two angle: Extrude in one direction as well as the opposite direction, where each direction has its own set of parameters (e.g., each direction has its own length).
• Through all: Extrude through everything (e.g., 360 angle).
• To first: Extrude until the first intersecting face.
• To face: Extrude until a specific face.

Angle and Two angle both enable the Reversed parameter, which reverses direction / directions of extrusion.

Angle and Through all both enable the Symmetric to plane parameter, which defines if the plane should be in the middle of the extrusion (extrude half-way outward from the sketch and extrude half-way inward from the sketch). This parameter is only available for Type of Angle.

Axis defines the axis from which the rotation happens:

• Vertical sketch axis / Horizontal sketch axis: The rotation happens using sketch's vertical / horizontal axis as the rotation axis.
• Construction line n: The rotation happens using construction geometry line in the sketch. Each line that is also construction geometry is listed.
• Base X-axis / Base Y-axis / Base Z-axis: The rotation happens using a basis axis as the rotation axis.
• Select reference: The rotation happens around a edge or datum line, which must be selected.

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Loft

An additive loft operation and a subtractive loft operation are the same thing, except that ...

• additive creates a solid and merges it with existing geometry it collides with.
• subtractive creates a solid and cuts out it from existing geometry it collides with.

A loft creates a solid by transitioning through sketches that act as slices within the solid. To loft a set of sketches, either ...

• use either toolbar button 11 (additive loft) or toolbar button 18 (subtractive loft), then ...
  1. select the loft's initial sketch in the Select Attachment pane that pops up and click OK,
  2. add the loft's subsequent sketches via the Add Segment button in the subsequent Loft Parameters pane that pops up (order of added sketches matter).
• select the sketches to loft and use either toolbar button 11 (additive loft) or toolbar button 18 (subtractive loft). The selection order of the sketches matters (e.g., first selected will become loft's initial sketch, second selected becomes the first transition sketch).

A loft's sketches must be spaced out. It's typically for all of a loft's sketches to be attached to the same face / plane, but each offset such there's gaps between them. A sketch can be offset and rotated relative to whatever surface it's attached to using its AttachmentOffset properties.

The Ruled surface parameter defines whether transitions between sketches are smooth or straight (straight if checked).

The Closed parameter makes a transition from the last sketch to the initial sketch, creating a loop.

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Pipe

An additive pipe operation and a subtractive pipe operation are the same thing, except that ...

• additive creates a solid and merges it with existing geometry it collides with.
• subtractive creates a solid and cuts out it from existing geometry it collides with.

A pipe creates a solid by transitioning through sketches in addition to following a chain of one or more paths (e.g., edge, arc, b-spline). To pipe a path and a set of sketches, either ...

• use either toolbar button 12 (additive pipe) or toolbar button 19 (subtractive pipe), then ...

  1. select the pipe's initial sketch in the Select Attachment pane that pops up and click OK,
  2. select the pipe's initial path in the Pipe Parameters by clicking the Object button within Path to Sweep Along and clicking the segment.

• select the initial sketch to pipe and the segment to follow, then use either toolbar button 11 (additive pipe) or toolbar button 18 (subtractive pipe). The selection order matters (e.g., first selected the sketch then select the segment).

The pipe can transition through multiple paths and many sketches:

• Add subsequent paths by clicking Add Edge and selecting the segment (order of edges matter).
• Add subsequent sketches by clicking Add Section and selecting the sketch (order of added sketches matter). Transform Mode must be Multisection for this to be enabled.

A pipe's sketches must be spaced out along the segments that make up the path, and the segments (lines, b-splines, etc..) that make up the path must be connected back-to-back. A common way to structure a pipe is to place sketches along a single b-spline. The b-spline can be created via the Part workbench or programmatically:

import FreeCAD as App
import Part

pts = [
    App.Vector(0,0,0),
    App.Vector(20,0,10),
    App.Vector(40,20,20),
    App.Vector(60,10,40),
]

curve = Part.BSplineCurve()
curve.interpolate(pts)

edge = curve.toShape()
wire = Part.Wire([edge])

obj = App.ActiveDocument.addObject("Part::Feature", "PipePath")
obj.Shape = wire
App.ActiveDocument.recompute()

Since the b-spline belongs to the Part workbench rather than the Part Design workbench, it lives outside of the Part Design body where the sketches live. It needs to be imported into that Part Design body using a subshape binder or as a base feature:

1. Ensure the body is active.
2. Select the b-spline.
3. Click subshape binder in the toolbar (green blob with 3 dots) to create a subshape binder object in the body.

Sketches can then be attached to the b-spline by attaching them to that subshape binder. Each attached sketch can be placed somewhere along the b-spline by setting the sketch's Map Path Parameter property (0.0 places at start, 1.0 places at end). The sketch's normal will follow the b-spline's trajectory at the position its at, but can also be further manipulated using the sketch's Attachment Offset property.

The Corner transition parameter defines how the path handles hard corners in the path:

• Transformed: Hard corners are automatically dealt with, potentially resulting in skewing, warping, and/or rotation.
• Right corner: Hard corners are not rounded (e.g., when the path goes from down to right at 90 degrees, it will abruptly change the profile, producing a hard cornered L shape).
• Rounded corner: Hard corners are rounded (e.g., when the path goes from down to right at 90 degrees, it will hold the inner in place and sweep the other end to produce a rounded shape).

The Orientation mode parameter defines how the profile rotates as it sweeps along the path:

• Standard: Orientation stays normal to path (normal vector).
• Fixed: Orientation keeps initial sketch's orientation. Cross-section shape will not rotate along with the path.
• Frenet: Orientation minimizes twisting.
• Auxiliary: Orientation is specified by a secondary path. For each point P along the path, there should be a point Q in the secondary path. As the profile is swept, the PQ line will be the normal of the swept path.
• Binormal: Orientation set to constant direction/vector as the orientation reference.

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Helix

An additive helix operation and a subtractive helix operation are the same thing, except that ...

• additive creates a solid and merges it with existing geometry it collides with.
• subtractive creates a solid and cuts out it from existing geometry it collides with.

A helix creates a solid by taking a sketch and rotating it up / down some axis, similar to the threads of a screw. To helix a sketch, either ...

• use either toolbar button 13 (additive helix) or toolbar button 20 (subtractive helix), then select the helix's initial sketch in the Select Attachment pane that pops up and click OK.
• select the sketch to helix, then use either toolbar button 13 (additive helix) or toolbar button 20 (subtractive helix).

The Axis parameter controls which axis to rotate around.

The Left handed parameter rotates in the opposite direction (to the left rather than the right).

The Reversed parameter flips the ascension in the opposite direction (descends the helix instead).

The Mode parameter defines how the ascension and rotation are configured. The values control which configuration fields show up:

• Pitch-Height-Angle

  • Pitch controls how far apart a full turn is (e.g., if the thread was 2mm wide and the pitch was 2mm there would be no space between threads vs if the thread was 2mm wide and the pitch was 4mm there would be 1 thread's worth of a gap between threads).
  • Height controls how far the helix ascends.
  • Angle controls tapering of the helix (negative degrees tapers inward vs positive degrees taper outwards).

  Some other options have a Turns parameter (number of full rotations). Turns is implicitly defined by Pitch and Height (e.g., pitch of 4mm at 8mm high is 2 turns).

• Pitch-Turns-Angle

  • Pitch controls how far apart a full turn is (e.g., if the thread was 2mm wide and the pitch was 2mm there would be no space between threads vs if the thread was 2mm wide and the pitch was 4mm there would be 1 thread's worth of a gap between threads).
  • Turns controls the number of full rotations.
  • Angle controls tapering of the helix (negative degrees tapers inward vs positive degrees taper outwards).

  There is no Height parameter here. Height is implicitly defined by Pitch and Turns (e.g., pitch of 4mm at 2 turns is 8mm high).

• Height-Turns-Angle:

  • Height controls how far the helix ascends.
  • Turns controls the number of full rotations.
  • Angle controls tapering of the helix (negative degrees tapers inward vs positive degrees taper outwards).

  There is no Pitch parameter here. Pitch is implicitly defined by Height and Turns (e.g., height of 8mm at 2 turns implies a pitch of 4mm).

• Height-Turns-Growth:

  • Height controls how far the helix ascends.
  • Turns controls the number of full rotations.
  • Growth controls how much the helix widens at the end of each turn.

  There is no Pitch parameter here. Pitch is implicitly defined by Height and Turns (e.g., height of 8mm at 2 turns implies a pitch of 4mm).

  There is no Angle parameter here. Angle is implicitly defined by Growth (translates the widening per turn to an angle).

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Primitives

An additive primitive and a subtractive primitive operation are the same thing, except that ...

• additive creates a solid and merges it with existing geometry it collides with.
• subtractive creates a solid and cuts out it from existing geometry it collides with.

A primitive is a primitive piece of 3D geometry (e.g., cube, sphere, torus). To create a primitive, use either toolbar button 14 (additive primitive) or toolbar button 21 (subtractive primitive) to show a drop-down of primitive types and select. Once selected, a Primitive Parameters pane will appear that defines the shape as well as a Select Attachment pane that defines how and what it attaches to. For full details, see sources.

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Fillet / Chamfer

Fillet / chamfer cuts into a edge. A fillet's cut is rounded while a chamfer's cut is straight.

To apply fillet/chamfer, select relevant faces and edges and use either toolbar button 23 (fillet) or toolbar button 24 (chamfer).

A Fillet Parameters / Chamfer Parameters pane will pop open. To add edges/faces, click Select, select the edges/face, and then click Confirm Selection. To remove edges/faces, click on the edge/face in the list and press Del.

For fillet, use the Radius field or the gizmos to set the radius of the curve.

For chamfer, use the Type or the gizmos to define how steep the the cut is:

• Equal distance sets the cut point equally away from both ends of the edge, defined by Size.
• Two distance sets the cut point for each edge, defined by Size and Size 2.
• Distance and angle sets the cut point for one side of the edge and uses an angle to determine the cut point of the other side of the edge, defined by Size and Angle.

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Draft

Draft adds an angle to one or more faces.

To apply draft, select relevant faces and use either toolbar button 25.

A Draft Parameters pane will pop open. To add faces, click Select, select the face, and then click Confirm Selection. To remove faces, click on the face in the list and press Del.

The Draft angle field sets the angle to offset the faces (can be negative).

The Neutral Plane field sets the plane in which the edge must be anchored (won't lift or sink). To set, click the button and select a face. In the example above, the neural plane is the top face. The 4 sides which have draft applied fan out toward the bottom because the top edges are locked in place.

The Pull Direction field sets the direction in which the angle is applied. To set, click the button and select an edge (or something edge-like, like a datum line?).

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Thickness

Thickness removes one or more faces and cuts out the inside of the object, giving it a bowl-like / shell-like effect.

To apply thickness, select relevant faces and use toolbar button 26.

A Thickness Parameters pane will pop open. To add faces, click Select, select the face, and then click Confirm Selection. To remove faces, click on the face in the list and press Del.

The Thickness field sets the thick the shell is. If Make thickness inwards is clicked, the original outline is kept but hollowed out vs padding the original outline to generate the shell.

The Mode field must be set to Skin.

The Join type field defines how non-tangential faces of the shell are joined together:

• Arc: Faces that do not intersect are joined by a fillet with a radius equal to Thickness value.
• Intersection: Faces that do not intersect are extended to meet at their virtual intersection.

The Intersection checkbox avoids self-intersection in some models.

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Boolean

Boolean moves one or more outside bodies into the active body and performs a boolean/set operation (union, intersection. subtraction).

To apply boolean, select relevant faces and use toolbar button 22. A Boolean Parameters pane will pop open.

To move a body into the active body, click Add Body and select the body. To move an added body back out, click Remove Body and select the body in Model pane.

The drop-down below the list of added bodies is the operation to perform:

• Common is intersection.
• Fuse is union.
• Cut is subtraction - the added bodies are subtracted from the active body.

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Mirror

Mirror copies either the entire body or specific features across a plane.

To apply mirror, use toolbar button 27. A Mirror Parameters pane will pop open.

Select Transform body for mirroring of the full model or Transform tool shapes to mirror specific features. If Transform tool shapes is selected, for each feature to mirror, click Add Feature and select the feature in the Model pane. Likewise, remove a feature being mirror by clicking Remove Feature and selecting the feature in the Model pane.

The Plane field selects the plane across which mirroring happens:

• Base planes (e.g., XY plane).
• Datum planes.
• Sketch axes and construction lines from any feature that's based off a sketch.

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Polar Pattern

Polar pattern copies either the entire body or specific features, multiple times around an axis.

To apply polar pattern, use toolbar button 29. A Polar Pattern Parameters pane will pop open.

Select Transform body for patterning of the full model or Transform tool shapes to pattern specific features. If Transform tool shapes is selected, for each feature to mirror, click Add Feature and select the feature in the Model pane. Likewise, remove a feature being mirror by clicking Remove Feature and selecting the feature in the Model pane.

The Axis field selects the axis across which copying happens:

• Basis (e.g., X axis).
• Datum lines.
• Sketch axes and construction lines from any feature that's based off a sketch.

When Mode is ...

• Extent, the Length field controls how much to rotate around the axis (e.g., 180 degrees, 360 degrees, 720 degrees) and Occurrences field controls the number of copies (evenly spaced out around the rotation).
• Spacing, the Spacing field controls how much space there is between copies (e.g., 60 degrees between copies) and Occurrences field controls the number of copies.

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Linear Pattern

Linear pattern copies either the entire body or specific features, multiple times in a straight line.

To apply linear pattern, use toolbar button 28. A Linear Pattern Parameters pane will pop open.

Select Transform body for patterning of the full model or Transform tool shapes to pattern specific features. If Transform tool shapes is selected, for each feature to mirror, click Add Feature and select the feature in the Model pane. Likewise, remove a feature being mirror by clicking Remove Feature and selecting the feature in the Model pane.

The Direction area selects the line across which copying happens:

• Basis (e.g., X axis).
• Datum lines.
• Sketch axes and construction lines from any feature that's based off a sketch.

When Mode is ...

• Extent, the Length field controls the total amount of distance and Occurrences field controls the number of copies (evenly spaced out across that distance).
• Spacing, the Spacing field controls how much space there is between copies (e.g., 10mm between copies) and Occurrences field controls the number of copies.

The Direction 2 checkbox displays a second Direction area, which is used to copy the copies from the first direction area. In the example screenshot, the first direction area produces 3 holes upward, while the second direction area places 3 copies of those 3 holes across, totalling 9 holes.

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Multi-Transform

Multi-transform is a container that can apply a chain of linear pattern, polar pattern, and mirror features. In addition, it can apply scaling to copies produced by these features.

To apply multi-transform, either ...

• use toolbar button 30.
• select existing linear pattern, polar pattern, and / or mirror features in the Model pane and use toolbar 30. The selected features will be imported into the multi-transform.

A Multi-Transform Parameters pane will pop open.

Select Transform body for patterning of the full model or Transform tool shapes to pattern specific features. If Transform tool shapes is selected, for each feature to mirror, click Add Feature and select the feature in the Model pane. Likewise, remove a feature being mirror by clicking Remove Feature and selecting the feature in the Model pane.

Right-click inside the Transformations list to add, delete, edit, and reorder transformations. The Scale transformation takes copies made in the previous transformation and applies compound scaling (e.g., first copy is 2x scaled, second copy, 3x scaled, etc..), as shown in the example. For copies of the body, this may work as intended. For copies of features, this may not work as intended (e.g., in the example screenshot, notice that the pockets don't seat on the face as they scale).

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Part Workbench

Part workbench allows building a 3D object through a hierarchy of transformations. In contrast to the part design workbench, the part workbench ....

• can produce both contiguous 3D objects and non-contiguous 3D objects (e.g., the 3D object can be comprised of multiple separated pieces, but it'll still be treated as a single 3D object).
• produces a 3D object through a hierarchy of transformations as opposed to a linear chain of 2D sketch to 3D feature.
• produces a 3D object outside of a container, meaning the operations / transformations don't need to nest in a container similar to part design's body.

The core components of the part workbench are geometry objects and compounds (a compound is a grouping of geometry objects, treated as a single piece of geometry). The workflow is to build out more complex pieces of geometry through transformations: Multiple pieces of existing geometry into one or more pieces of new geometry (e.g., boolean intersection, converting two 2D lines to a ruled surface, sweeping over profiles).

User Interface

Geometry Creation

• (1) Geometry creation: These toolbar buttons create standard geometry out of nothing other than user parameters. Geometry may be solids, surfaces, of profiles (e.g., 2D coplanar geometry). From left-to-right, ...

  • create a cube.
  • create a cylinder.
  • create a sphere.
  • create a cone.
  • create a torus.
  • create a tube.
  • create a one of many types of standard shapes / geometric primitives (e..g, cube, prism, plane, circle, line, vertex).

• (3) Create a sketch (either on plane or face).

Geometry Transformation

• (2) Shape Builder: Creates complex shapes from geometric primitives.

• (4) Basic transformations: These toolbar buttons create manipulate and transform geometry. From left-to-right, ...

  • extrude a profile.
  • revolve a profile.
  • mirror geometry.
  • scale geometry.
  • fillet edges.
  • chamfer edges.
  • create face from wires (e.g., from a sketch).
  • create a ruled surface between two wires.
  • loft through a set of profiles.
  • sweep through a set of profiles.
  • boolean intersection two objects, as wire geometry.
  • create wireframe cross sections from an exist 3D object.
  • drop-down to either ...
    • fatten a 3D object.
    • fatten a profile.
  • convert a 3D object to a shell, leaving selected faces open.
  • project edges/wires/faces of one object onto another.
  • change appearance of a face.

• (5) Boolean operations: These toolbar buttons transform multiple pieces of geometry. From left-to-right, ...

  • drop-down to either ...
    • group together (compound) several pieces of geometry (not a boolean union, restrictions apply).
    • break apart a compound back to its individual parts.
    • break out some geometry in a compound, using filters.
  • boolean operation between two 3D objects (e.g., union, intersection, difference).
  • boolean difference a 3D object from another.
  • boolean union two 3D objects.
  • boolean intersect two 3D objects.
  • drop-down to either ...
    • boolean union two walled / hollowed 3D objects, preserving voids.
    • boolean union two walled / hollowed 3D objects, preserving voids on one of the objects.
    • boolean difference two walled / hollowed 3D objects, making sure to remove the void as well.
  • drop-down to either ...
    • splits two 3D objects into it's boolean differences (both A-B and B-A) and boolean intersection, under a compound. The compound of differences and intersection together form the boolean union.
    • splits a 3D object using another 3D object as a "cutter", resulting in its boolean difference (A-B only) and boolean intersection. The split pieces are placed as individual 3D objects, not under a compound.
    • splits a 3D object using another 3D object as a "cutter", resulting in its boolean difference (A-B only) and boolean intersection. The split pieces under a compound.
    • boolean XOR two 3D objects, effectively removing the boolean intersection ([A-B]∪[B-A])

• (7) Defeaturing: Removes certain features of a 3D object (e.g. holes, chamfers, edges_FC), to fix defects and simplify.

Helpers

• (6) Check geometry: analyze selected geometry for errors.

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Organization

The core components of the Part workbench are geometry and compounds. A compound is a grouping of a geometry objects, treated as a single geometry object.

A geometry object could be ...

• a primitive (e.g., cube, line, cone, vertex).
• the result of some transformation (e.g., boolean intersection of two objects, filleting an edge).
• the combination of geometry objects (e.g., compoun_FCd object).
• a body.

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Geometry

A geometry object contains some geometry and has a local coordinate system to place and orient it in relation to the parent's coordinate system.

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Compound

A compound is a set of geometry objects brought together under a single container, where that container itself is a geometry object. A compound is not a boolean operation - objects remain separate as opposed to being merged together in together.

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Part Design Interoperability

Part Design Workbench to Part Workbench

A part design body can naturally be operated on by the part workbench. For example, the part workbench can boolean union a body with a cube generated from within the part workbench.

Part Workbench to Part Design Workbench

A part workbench object cannot naturally be operated on by the part design workbench. The object must be pulled into the body either using a subshape binder or as a base feature.

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Primitive

Include anything that builds solids

Ruled Surface

Face from Wires

Shape Builder

Profile Transformations

Mirror, revolve, pad

Chamfer / Fillet

Boolean Operations

Profile Operations

Fattening Operations

Thickness / 2D offset / 3D offset

Assembly Workbench

Assembly workbench allows linking individual models by specifying how they fit and move together. For example, a piston and its enclosure can be linked together such that piston moves up and down its enclosure.

The core component of the assembly workbench is the joint. A joint positions and restricts the degrees of freedom a model has in relation to some other model.

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User Interface

Assembly

• (1) Create new assembly.
• (2) Add component (may be a model or a standard part_FC).
• (3) Solve assembly.
• (4) Explode view of assembly.
• (5) Simulation of assembly.
• (6) Bill of materials.

Joints

• (7) Joint types: These toolbar buttons give quick access to joints functionality. From left-to-right, ...

  • create grounded joint, locking a component into place.
  • create fixed joint, locking a component relative to another component.
  • create revolute joint, locking a component's movement such it only revolves around some axis.
  • create cylindrical joint, locking a component's movement such it only revolves and slides along some axis (combination of slider joint and revolute joint).
  • create slider joint, locking a component's movement such that it only slides along some axis.
  • create ball joint, locking a component_FC's movement to a specific point, allowing unrestricted movement so long as it touches that point.
  • create distance joint, locking the movement of two components to be a specific distance from each other.
  • create parallel joint, locking the movement of two components such that their z-axis are parallel.
  • create perpendicular joint, locking the movement of two components such that their z-axis are perpendicular.
  • create angle joint, locking the movement of two components such that their z-axis are fixed at a specific angle.
  • create rack and pinion joint, locking a component with a sliding joint around a component with a revolute joint.
  • create screw joint, locking a component with a sliding joint around a component with a revolute joint.
  • drop-down to either ...
    • create gear joint, locking two components with revolute joints together, with opposite rotating direction.
    • belt joint locks_FC, locking two rotating components with revolute joints together, with same rotation direction.

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Organization

The core pieces of the assembly workbench are components and joints. A component is an app link to either a model or a standard part_FC containing a group of models. A joint is a linkage between components that restricts its positioning, orientation, and / or movement (e.g., restricts its degrees of freedom). For example, a slider joint locks one component to another, restricting its movement such that it can only slide along some axis on that / derived from that component.

• A joint constrains the movement of one or more components, often relative to each other.
• A component can be constrained by by zero or more joints.

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Assembly

An assembly is a container of that ties together models (e.g., bodies, standard parts_FC containing bodies) with joints, defining how those models move in relation to each other. An assembly can also contain sub-assemblies. A sub-assembly is an assembly that's nested within another assembly.

To create an assembly, use toolbar button 1 (keyboard shortcut A). Assemblies can be created at the top-level, within an existing assembly (in which case it's referred to as a sub-assembly), or even within a standard part_FC.

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Component

A component is a non-joint object within an assembly (e.g., body, standard part_FC, sub-assemblies).

To insert a component, use toolbar button 2 and select Component (keyboard shortcut I). An Insert pane should appear with options to insert one or more components or sub-assemblies.

Clicking objects in the drop-down imports them into the assembly. Importable objects include models, standard parts_FC, and assemblies (become sub-assemblies in the assembly being imported into). Each object imported is imported as a reference as opposed to a copy, meaning changes in the source will reflect in the assembly.

Above the list is a text field that filters items in the list.

Below the field is ...

• the button Open File, which opens a file to introduce new objects.
• the checkbox Show only parts, which filters the list of objects to standard parts_FC and assemblies.
• the checkbox Rigid sub-assemblies, which imports assemblies without joint movements enabled.

If the object being imported is the first object, a prompt will show up asking if the object should be locked into place with a grounded joint. An assembly needs at least one grounded joint on which other joints and objects are anchored.

A component can be moved by left mouse button dragging in the 3D viewport. If movement is constrained by joints, only allowed movements are applied during dragging.

If a component is not constrained by joints, selecting it presents a gizmo that can be used to move it around. A sub-assembly that's rigid is always moved as a whole, while a sub-assembly that isn't rigid can have its individual components separated and moved.

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Joint

A joint constrains the movement of one or more components, often relative to each other.

There are many types of joints, starting from toolbar button 7 onward. An assembly needs at least one grounded joint on which other joints and objects are anchored.

Each individual joint type is documented in further detail in sections further down.

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Frame

A frame binds a component's element (e.g., face, plane, vertex) to a joint, providing that element with its own local coordinate system. A joint restrict the movement of its frames (and thereby the components those frames are attached to) based on that joint's type and parameters.

A frame is visualized in the viewport as a white transparent disc:

• The white disc represents a frame's XY plane.
• The red line to the side of the white disc represents that frame's X-axis.
• The green line to the side of the white disc represents that frame's Y-axis.
• The blue line coming out from the white disc's center represents that frame's z-axis / plane normal.

The joint in the example below is a sliding joint. A sliding joint has two frames, restricted such that the frames are parallel to each other and the only movement/rotation change allowed is sliding up-and-down the z-axis.

Joints

The subsections below detail joint types supported by the assembly workbench. Most joints present a configuration pane during creation with a constant subset of options.

• (1) Joint type: Joint being applied. The joint type can be changed by using this drop-down. Some joints types may not be available (e.g., grounded joint).

  ⚠️NOTE️️️⚠️

  Sometimes, changing this value doesn't work. The joint will show up as the selected type but it won't be applied.

  Noted in v1.1.1.

• (2) Model elements: Model elements (e.g., faces, edges, vertices) which the joint applies to.

• (3) Configuration: Configuration options for the select joint type. Options differ per joint type.

• (4) Isolate: Controls how unrelated components appear when the joint is selected:

  • Transparent views unrelated components partially transparent.
  • Wireframe views unrelated components as wireframe.
  • Hidden removes unrelated components from view.
  • Disabled keeps unrelated components in view as-is.

  

When offset and rotation parameters don't specify a relation (as in the example above), many joint types apply it to the z-axis of one of their frame's local coordinate systems. In the example above, the offset parameter of 7mm is applied to the second frame's local coordinate system's z-axis.

Often times, it's possible to offset and rotate in more directions by selecting Show advanced offsets (or some equivalent checkbox / button). In the example above, selecting Show advanced offsets replaces the Offset and Rotation fields with Offset1 and Offset2. These new fields directly control the offset and rotation for their respective frames's local coordinate system.

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Grounded Joint

A grounded joint locks the location and orientation of an assembly piece. A non-empty assembly needs to have at least one grounded joint.

To apply a grounded joint, select the component and select toolbar button 7 (keyboard shortcut G). Doing this multiple times toggles the grounded joint on and off.

Once a grounded joint is applied, a red lock will appear over the piece.

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Fixed Joint

A fixed joint locks one component onto another component, preventing any movement or rotation.

To apply a fixed joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 8 (keyboard shortcut F).
• select toolbar button 8 (keyboard shortcut F), then select two elements (e.g., edge, face, vertex), one on each component.

• Offset: Translates joint's second frame's LCS's z-axis.
• Rotation: Rotates around the joint's second frame's LCS's z-axis.
• Up/down button: Flips joint's LCS such that the z-axis points in the opposite direction.

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Revolute Joint

A revolute joint allows the rotation of one component around another component using the shared z-axis between both frames. All other movements and rotations are restricted.

To apply a revolute joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 9 (keyboard shortcut R).
• select toolbar button 9 (keyboard shortcut R), then select two elements (e.g., edge, face, vertex), one on each component.

A revolute joint lines matches up both frames and rotates around the shared z-axis.

• Offset: Translates joint's second frame's LCS's z-axis.
• Up/down button: Flips joint's LCS such that the normal points in the opposite direction.
• Min angle / Max angle: If enabled, restricts the rotational angle range.

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Slider Joint

A slider joint allows the sliding of one component along another component using the shared z-axis between both frames. All other movement and rotation are restricted.

To apply a slider joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 11 (keyboard shortcut S).
• select toolbar button 11 (keyboard shortcut S), then select two elements (e.g., edge, face, vertex), one on each component.

• Rotation: Rotates around the joint's second frame's LCS's z-axis.
• Up/down button: Flips joint's LCS such that the normal points in the opposite direction.
• Min length / Max length: If enabled, restricts how far the two frames can extend out in either direction.

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Cylindrical Joint

A cylindrical joint is a combination of the slider joint and revolute joint. Both sliding and rotation are allowed (matching the allowed movement/rotation of both slider joint and revolute joint), but all other movements and rotations are restricted.

To apply a cylindrical joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 10 (keyboard shortcut C).
• select toolbar button 10 (keyboard shortcut C), then select two elements (e.g., edge, face, vertex), one on each component.

• Up/down button: Flips joint's LCS such that the normal points in the opposite direction.
• Min length / Max length: If enabled, restricts how far the two frames can extend out in either direction.
• Min angle / Max angle: If enabled, restricts the rotational angle range.

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Ball Joint

A ball joint allows the movement of one component relative to another component so long as the center of those components's frames are touching.

To apply a ball joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 112(keyboard shortcut B).
• select toolbar button 12 (keyboard shortcut B), then select two elements (e.g., edge, face, vertex), one on each component.

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Distance Joint

A distance joint allows the movement of one component relative to another component so long as the distance between them is some constant.

To apply a distance joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 13 (keyboard shortcut D).
• select toolbar button 13 (keyboard shortcut D), then select two elements (e.g., edge, face, vertex), one on each component.

• Distance: Distance between frames.
• Up/down button: Flips joint's LCS such that the normal points in the opposite direction.

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Parallel Joint

A parallel joint allows the movement of one component relative to another component so long as those components's frames have parallel planes.

To apply a parallel joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 14(keyboard shortcut N).
• select toolbar button 14 (keyboard shortcut N), then select two elements (e.g., edge, face, vertex), one on each component.

• Up/down button: Flips joint's LCS such that the normal points in the opposite direction.

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Perpendicular Joint

A perpendicular joint allows the movement of one component relative to another component so long as those components's frames have perpendicular planes.

To apply a perpendicular joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 15 (keyboard shortcut M).
• select toolbar button 15 (keyboard shortcut M), then select two elements (e.g., edge, face, vertex), one on each component.

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Angle Joint

An angle joint allows the movement of one component relative to another component so long as those components's frames have normals at some constant angle.

To apply a angle joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 16 (keyboard shortcut X).
• select toolbar button 16 (keyboard shortcut X), then select two elements (e.g., edge, face, vertex), one on each component.

• Angle: Angle between the frame normals.

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Rack and Pinion Joint

A rack and pinion joint ties together a slider joint and a revolute joint, such that rotation of that revolve joint results in sliding of the slider joint and vice versa. This gives the impression of a cog/pinion moving across a rack.

Prior to applying a rack and pinion joint, ensure that ...

1. there's a component with a sliding joint.
2. there's a component with a revolute joint.

To apply a rack and pinion joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 17 (keyboard shortcut Q).
• select toolbar button 17 (keyboard shortcut Q), then select two elements (e.g., edge, face, vertex), one on each component.

One element must be on a component that is sliding (e.g., the rack), while the second element must be on the revolving component (e.g., pinion). The normals of the 2 frames must be perpendicular to each other (blue lines must be 90 degrees).

Pitch radius: The contact radius of the revolving component against the rack component.

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Screw Joint

A screw joint ties together a slider joint and a revolute joint, such that sliding the slider joint revolves the revolute joint. This gives the impression of a screw turning as it goes down.

Prior to applying a screw joint, ensure that ...

1. there's a component with a sliding joint.
2. there's a component with a revolute joint rotating along the same axis that sliding is occurring on.

To apply a screw joint, either ...

• select two elements (e.g., edge, face, vertex), one on each component, and then select toolbar button 18 (keyboard shortcut W).
• select toolbar button 18 (keyboard shortcut W), then select two elements (e.g., edge, face, vertex), one on each component.

One element must be on a component that the sliding joint is sliding in/out of (e.g., screw hole), while the second element must be on the revolving component (e.g., screw). The normals of the 2 frames must be pointing at each other (blue lines must be facing each other).

Once applied, sliding will also result in revolving.

Thread pitch: The thread pitch of the revolving component representing the screw (distance the screw advances in 1 full turn).

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Gear / Belt Joint

A gear / belt joint ties two revolute joints together, such that revolving one automatically revolves the other. This gives the impression of one gear moving another. A gear joint revolves in opposite directions while a belt joint revolves in the same direction.

Prior to applying a gear / belt joint, ensure that there two components each with a revolute joint whose frame normal points in the same direction / opposite direction. To apply a gear / belt joint, either ...

• select two elements - the element that each component has its revolve joint on. Then, select toolbar button 19's drop-down and select either gear joint (keyboard shortcut T) or belt joint (keyboard shortcut L).
• select toolbar button 19's drop-down and select either gear joint (keyboard shortcut T) or belt joint (keyboard shortcut L). Then, select two elements - the element that each component has its revolve joint on.

Reverse rotation: Swaps the joint type between Gears and Belt. The only difference between them is if the direction is reversed

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Exploded View

An exploded view of an assembly is the components of that assembly fanned out, for presentation purposes.

To create an exploded view, select toolbar button 4 (keyboard shortcut E). An Explode Views pop-out will appear in addition to a !!Exploded_Views!! container. An assembly can hold multiple exploded views, all all of which live under that assembly's single Exploded_Views container.

• The list within the Exploded Views pop-out is a sequence of move operations. There are multi ways to move:

  • Selecting a single component in the 3D viewport exposes a gizmo which can move and rotate that component. Each move on a component generates a single "Move" item in the list along with a dashed red line tracing that move, as shown in the example above.

  • Selecting multiple components in the 3D viewport exposes a single gizmo which can move and rotate those components in tandem. Each move on the set of components generates a single "Move" item in the list (e.g., even though multiple components are being moved, a single "Move" item is generated) along with multiple dashed red line tracing the moves of the individual components.

    

  • Clicking Explode Radially exposes a single gizmo at the center of the assembly which can move and rotate all components in tandem. Moving fans out the components circularly. Each move on the set of components generates a single "Move" item in the list (e.g., even though multiple components are being moved, a single "Move" item is generated) along with multiple dashed red line tracing the moves of the individual components.

    

• Align dragger to...: Moves the gizmo to a different location, such as the origin, center, or to a specific component if multiple components are selected for moving.

  ⚠️NOTE️️️⚠️

  Moving to a different component seems bugged in FreeCAD 1.1.1. It doesn't actually move, and if you look at the logs it keeps spamming class 'TypeError'.

• Parts as a single solid: Treats components that are standard parts_FC as a single solid.

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Bill of Materials

A bill of materials (BOM_FC) of an assembly is the list of that assembly's components as well as optionally its sub-components, such as sub-assemblies and the constituent pieces of a standard part_FC.

To create an BOM_FC, select toolbar button 6 (keyboard shortcut O). A Bill of materials pop-out will appear.

• Sub-assemblies children: If selected, includes children of sub-assemblies in the BOM_FC.

• Parts children: If selected, includes children of standard parts_FC in the BOM_FC.

• Only parts: If selected, includes only standard parts_FC and sub-assemblies in the BOM_FC, skipping other objects (e.g., bodies).

• Columns: Columns to be included in the BOM_FC. New columns can be added by clicking the Add Column button, which injects a text field into the list to be filled out. A column will target an object property if it starts with with a period. For example, .Visibility pulls in the Base.Visibility property from each listed object's data properties.

  

  ⚠️NOTE️️️⚠️

  The example property above exists for nearly all 3D objects, found in the Model pane's data properties section. It might not appear because it's hidden - right-click and select "Show hidden" to see it.

  ⚠️NOTE️️️⚠️

  I've tried targeting properties outside of Base. It doesn't seem to work. The only properties you can target seem to be those under Base. Note that you can inject custom properties by right-clicking in the properties and selecting Add Property, and then pull in that custom property to a BOM_FC column.

Clicking OK generates the spreadsheet containing the BOM_FC. If the active object is an assembly, the BOM_FC is generated for that assembly under a Bill_of_Materials container. Otherwise, the BOM_FC is generated as a top-level objects for all assemblies in the document (one BOM_FC covering all assemblies).

Similarly, clicking Export saves the BOM_FC as a tab-separated text file (TSV).

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Simulation

A simulation updates the motion state of one or more of an assembly's joints across some duration of time, resulting in simulated movement. The motion state of the joint is a function of time elapsed (e.g., for a duration of 5 seconds, a revolute joint's angle should be 5*time).

To create an simulation, select toolbar button 7 (keyboard shortcut V). A simulation gets placed under the assembly's Simulations container and a Simulations pop-out will appear.

• Motions: The joints to which motion are to be applied to. To add a joint, use the green plus button to open a selection pop-out.

  

  Use Joint to target the joint to apply motion to, and Motion type to apply the target the type of motion. Some joints support multiple types of motion (e.g., a cylindrical joint supports both sliding and rotating), but most joints only support one type of motion.

  Formula is the expression used to update the motion state of the joint. The motion is a function of time elapsed across a duration (e.g., for a duration of 5 seconds, a revolute joint's angle should be 5*time). The Help button extends the pop-out to give examples of formulas.

• Simulation Settings: The duration and cadence across which motion occurs:

  Start / Stop: Duration, specified as a start and stop time. Step: How often to update the motion state (e.g., if the duration is 5s and the step value is 1s, the motion's state will be updated once a second).

  ⚠️NOTE️️️⚠️

  What is Tolerance? I'm not sure. AI is saying that it's the tolerance of the assembly workbench's numerical solver - how close it has to get to solution before it considers it solved. I couldn't find anything in the documentation or forums corroborating this.

  Best not to mess with the default.

Once Motions and Simulation Settings have been defined, the Generate button produces an animation scrubber that can be used to play and scrub through the simulation. Updates to Motion and / or Simulation Settings require the Generate button to be pressed again for the scrubber to update.

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Datum Geometry

Datum geometry are helper primitives typically used to position other objects (e.g., sketches, features, bodies in an assembly), similar to construction geometry in sketches. Datum geometry aren't unique to a specific workbench.

Datum geometry can inserted using the toolbar button next to the button that creates a new standard part_FC.

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Datum Point

A datum point commonly needs one or more objects to define its attachment / positioning (e.g., faces, lines, vertices). To insert a datum point, either ...

• select the objects to attach the datum point to, then select the Datum Point toolbar button.
• deselect everything, select the Datum Point toolbar button, then individually reference objects in the Attachment pane pop-up by clicking a Reference button and selecting the entity.

The Attachment mode parameter defines what types of objects are needed for positioning / attachment (hovering over an option describes what it does as well as supported reference types). Once attached, the Attachment offset parameters tweak the position by offsetting and a rotation.

The example above attaches the datum point to a vertex and then positionally offsets itself.

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Datum Line

A datum line typically needs one or more objects to define its attachment / positioning (e.g., faces, lines, vertices). To insert a datum line, either ...

• select the objects to attach the datum line to, then select the Datum Line toolbar button.
• deselect everything, select the Datum Line toolbar button, then individually reference objects in the Attachment pane pop-up by clicking a Reference button and selecting the entity.

The Attachment mode parameter defines what types of objects are needed for positioning / attachment (hovering over an option describes what it does as well as supported reference types). Once attached, the Attachment offset parameters tweak the position by offsetting and a rotation.

The example above attaches the datum line to 2 datum points, defining that line.

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Datum Plane

A datum plane needs one or more objects to define its attachment / positioning (e.g., faces, lines, vertices). To insert a datum line, either ...

• select the objects to attach the datum plane to, then select the Datum Plane toolbar button.
• deselect everything, select the Datum Plane toolbar button, then individually reference objects in the Attachment pane pop-up by clicking a Reference button and selecting the entity.

The Attachment mode parameter defines what types of objects are needed for positioning / attachment (hovering over an option describes what it does as well as supported reference types). Once attached, the Attachment offset parameters tweak the position by offsetting and a rotation.

The example above attaches the datum plane to a vertex (origin) and 2 edges (normal vector and Y vector), defining that plane.

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Local Coordinate System

A local coordinate system is a frame of reference, defining it's own origin and basis axes relative to the parent origin and basis axes. A local coordinate system needs one or more objects to define its attachment / positioning (e.g., faces, lines, vertices). To insert a datum line, either ...

• select the objects to attach the datum plane to, then select the Datum Plane toolbar button.
• deselect everything, select the Datum Plane toolbar button, then individually reference objects in the Attachment pane pop-up by clicking a Reference button and selecting the entity.

Many objects come with their own builtin local coordinate system (e.g., a prism may have its own local coordinate system, where the vertexes of the prism are defined related to that local coordinate system). Objects may also be attached to local coordinate system (or some other object with a builtin local coordinate system), such that their position and/or orientation are relative to the local coordinate system (Attachment Mode property). _{[src] [src]}

Standard Part

A standard part_FC is a container that holds multiple 3D objects (e.g., bodies, assemblies), treating the collection of 3D objects as a single unit. A standard part_FC has its own local coordinate system so that objects within it are positioned and rotated relative to that local coordinate system, but externally the standard part_FC (and everything within it) is moveable and rotatable as a single unit.

Standard parts_FC aren't unique to a specific workbench.

To create a standard part_FC, use toolbar button 1. Objects can be moved in to / out of the standard part_FC by dragging them within the Model pane.

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Standard Group

A standard group_FC is a general purpose container that holds multiple objects of any type (e.g., spreadsheets, bodies, standard parts_FC). Standard groups_FC are typically used to hierarchically organize objects together, similar to a files and folders in a filesystem.

Standard groups_FC aren't unique to any specific workbench.

To create a standard group_FC, use the toolbar button that's immediately to the right of toolbar button 2 (folder icon). Objects can be moved in to / out of the standard group_FC by dragging them within the Model pane.

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App Link

An app link is an object that links to another object, intended to efficiently duplicate a single object multiple times.

App links aren't unique to any specific workbench.

To create an app link, use the toolbar button that's 2 to the right of toolbar button 2 (rounded rectangle with green arrow icon). An app link inherits the referenced object's icon and adds a small arrow to lower left to identify that it's an app link. It's Data properties will also contain a Link section, objects that are all links_FC have

• Linked Object: Object being referenced by this app link.

• Link Transform: Flag controlling whether to inherit Linked Object's Placement as this app link's Placement.

  • When true, inherit's Linked Object's Placement as this app link's Placement and instead exposes a Link Placement property in its place.
  • When false, overrides Linked Object's Placement with its own Placement property.

• Element Count and Show Element: The number of duplicates produced by this app link and how they're presented in the hierarchy.

  • When Element Count == 0, Linked Object is duplicated exactly once and this app link's children will mirror Linked Object's children.
  • When Element Count > 0 and Show Element is true, Linked Object is duplicated Element Count times and this app link will have Element Count children where each child is a link to Linked Object.
  • When Element Count > 0 and Show Element is false, Linked Object is duplicated Element Count times and this app link will have a single child linking to Linked Object.

• Link Execute: Python function to run anytime the link is recomputed.

• Link Copy On Change: Copy-on-write behavior.

  • When Disabled, this app link acts as a link: Changes to Linked Object are reflected in this app link and vice versa.
  • When Enabled, this app link acts as a link until it's changed: Changes to Linked Object are reflected in this app link until a "CopyOnChange" property is updated on this app link, at which point Link Copy On Change switches to Owned (changes to copied instead of linked). To mark/unmark a property as "CopyOnChange", right-click on it within the Model pane's Data panel, navigate to Status, and either select or unselect CopyOnChange.
  • When Owned, this app link is a deep copy of Linked Object rather than a link.
  • When Tracked, this app link is a deep copy of Linked Object rather than a link but attempts to keep non-modified properties in sync with future edits made to Linked Object.

• Scale: Uniform scaling factor that applies to all duplicates.

• Scale List: Per-axis scaling factor applied to each duplicate of Element Count (e.g., x scaling, y scaling, z, scaling). Only applicable if Element Count > 0.

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Variable Sets

Quality-of-Life Settings

The following sections highlight several settings to improve quality-of-life.

Enable dark mode:

The following instructions enable dark mode.

1. Go to Edit → Preferences → General → General and set Theme to FreeCAD Dark.

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Easier selections using trackpad

The following instructions make it easier to select items using a trackpad, where you don't have the same level of precision as a mouse.

1. Go to Edit → Preferences → Display → 3D View and set Marker size to 11 px.
2. Go to Edit → Preferences → General → Selection and set Radius to 11 px.
3. Go to Edit → Preferences → Sketcher → Appearance and set all line widths to 4 px (these seem to just be for elements, not constraints?).
4. Go to Edit → Preferences → Part Design → Shape Appearance and set Vertex Size to 9 px (can't seem to go till 11).
5. Go to Edit → Preferences → Part Design → Shape Appearance and set Line Width to 4 px.

Rotate at point

The following instructions make it so that rotation happens at where your mouse cursor is at, not at the viewport center.

1. Go to Edit → Preferences → Display → Navigation → Navigation and set Rotation mode to Drag at cursor.