Workarounds

Introduction

The goal of this article is to list some currently missing features in FreeCAD and provide workarounds for them. It can be helpful for new users who can't find a particular functionality in FreeCAD.

Workarounds for the Sketcher Workbench

No.	Missing feature	Workarounds
1	Auto snap to objects (midpoints, geometric centers, quadrants, extensions, intersections)	Manually apply constraints and use construction lines Draw geometry in the Draft Workbench, where snapping to objects is available, then convert to sketch with the Draft Draft2Sketch tool Midpoint snap is available within the Sketcher Snap option but doesn't apply any constraints
2	Chamfer tool	Make chamfers on the part level (after the sketch has been turned into a solid) with PartDesign Chamfer or Part Chamfer Create a fillet, change the arc to construction geometry and then connect the points with a line to create a chamfer Draw chamfers manually with lines or polylines
3	Circular pattern	Create circular patterns on the part level (after the sketch has been turned into a solid): For a PartDesign Workbench Feature use PartDesign PolarPattern For a Part Workbench shape, or a complete PartDesign Body, use Draft PolarArray or Draft CircularArray Use Draft PolarArray, then convert back to sketch with the Draft Draft2Sketch tool Position sketch features in a circular pattern manually, vertices of a polygon with a number of sides corresponding to the number of circular pattern instances or symmetry with respect to radially positioned construction lines can make it easier
4	Offset tool	SketcherOffset macro Part Offset2D tool (SubShapeBinder necessary for use in a PartDesign Body) Draft Offset tool (SubShapeBinder necessary for use in a PartDesign Body) Draw offset geometry manually, construction lines connecting the original and offset geometry and perpendicular to them at different locations, dimensioned with distance dimension will ensure proper relation between the geometries
5	Rotate tool	To rotate the whole sketch: change its Placement property To rotate a selection inside the active sketch: Remove constraints that prevent the rotation, e.g. with Sketcher RemoveAxesAlignment Optionally add constraints between the objects to be rotated Apply an appropriate Sketcher ConstrainAngle constraint or drag a vertex of one of the objects
6	Scale tool	Draft Scale, then Draft Draft2Sketch
7	Adaptive dimension constraint	Use a range of dimensional constraints: 3 for lines, 1 for angles and 3 for arcs/circles
8	Input coordinates and dimensions on the go (when drawing an object)	Apply dimensional constraints after drawing the geometry
9	Tangency to B-spline edge	Apply tangency to endpoints instead of edges
10	Check geometric and mass properties of the sketch (area, center of mass, second moments of area and so on)	Create a face from the sketch with Part MakeFace, then analyze that face with Part CheckGeometry
11	Possibility to use the results of the External Geometry tool directly for operations on the sketch	Manually trace over the geometry created by this tool Link Branch - Defining Geometry tool
12	Project multiple edges at once with the External Geometry tool when a face is selected	Project edges individually
13	3D sketches	Use the Draft Workbench, but 3D drafts can't be converted to sketches (however, they can be used for spatial frame analyses done internally or externally, and for PartDesign AdditivePipe or Part Sweep paths)
14	Projection of cut edges when making a sketch on a plane cutting through an object	Create a Link from the object, and slice that object to get actual cut edges
15	View section tool showing filled cuts	If the sketch is plane-parallel to one of the main planes of the global coordinate system: use Part SectionCut
16	Rectangle from 3 corners and rectangle from 3 points by center tools	Use the currently available rectangle from 2 opposite corners and rectangle from center tools and apply proper constraints afterwards
17	Diameter dimension with respect to a symmetry axis for revolved parts	Create a radius dimension instead (you can enter the diameter divided by 2 - the calculation will be handled by FreeCAD)
18	Curved slot tool	Draw curved slots manually Use one of the macros and scripts listed here
19	Dimension labels adapting to the rotation of the view to be always readable	Rotate the view when needed
20	First dimension in the sketch scaling the geometry so that its initially drawn shape is not broken	Apply some dimensional constraints before drawing the entire shape
21	An option to hide the whole construction geometry in an active sketch	In the Elements window, use the Construction filter, select the construction geometry entities there and uncheck their checkboxes

Workarounds for the Part Workbench and Part Design Workbench

No.	Missing feature	Workarounds
1	Check the geometric and mass properties of the model	FCInfo macro Part CheckGeometry tool – area, volume, mass, length, center of mass, moments of inertia, radius of gyration
2	Display the center of mass of the model (part or assembly)	Macro CenterOfMass
3	Clipping plane that doesn't make the model look like it's hollow	Change the Lighting property in the part's view settings to "One side" (very rough equivalent, problem with multicolored parts) Persistent section cut tool - deselect all planes before pressing Close Link Branch - experimental renderer
4	Creation of an axis on the intersection of 2 planes and a plane midway between two faces/points, possibly more variants for datum creation	Macro Intersection Manual adjustment of datum attachment
5	Automated midsurface extraction (for thin-walled parts)	Use Draft Facebinder and then Draft Scale or Part Offset (easier) to make it actual midsurface, apply the workaround for extending faces if the generated midsurfaces are separated and join them with boolean tools
6	Project (map/wrap) sketches on non-planar (e.g. cylindrical) faces	Curves SketchOnSurface tool in add-on Curves Workbench Part ProjectionOnSurface tool
7	Support for multiple solids within a body	Create a separate body for each solid Link Branch
8	Select which part of the sketch to pad	Select edges from the sketch and create a SubLink or a SubShapeBinder and pad that new object Pad a complete sketch located on the existing face of the model in the opposite direction (towards the existing shape) so that only new faces are created. Then it is possible to select these faces individually and pad them. This method should be used with caution since unnecessary 3D operations may lead to unexpected errors. Thus, it is recommended to use the previous workaround instead. Link Branch - Export Single Geometry and Export Multiple Geometries tools or automatic SubShapeBinder created when edges forming a closed loop are selected from the sketch before padding
9	Fillets and chamfers that can consume adjacent faces/edges	Make fillets with a slightly smaller radius (e.g. 6.4999 instead of 6.5 mm) Model these features directly using other operations, such as PartDesign Pocket or already include them in the sketches
10	Variable radius for the PartDesign Fillet tool	Use the Part Fillet tool which supports a variable radius
11	Parametric curves	Macro 3D Parametric Curve
12	Cosmetic threads	Add cosmetic threads on the TechDraw page Model true threads, for holes those can be generated automatically using the Hole tool
13	Partitions (splitting surfaces and volumes with sketches and datum planes while keeping the number of parts unchanged)	Boolean Fragments tool – only splitting surfaces with sketches
14	Guide rails for Additive Pipe and Additive Loft or their equivalents in the Part Workbench	Add-on CurvedShapes Workbench - CurvedArray or CurvedPathArray Add-on Curves Workbench - GordonSurface or Pipeshell Surface Workbench - Filling
15	Twist for PartDesign AdditivePipe or Part Sweep	PartDesign AdditiveHelix (pitch = height * 360 / twist angle) Add-on CurvedShapes Workbench - CurvedArray Multisection mode in Additive Pipe
16	Bending existing parts	For sheet metal objects: add-on SheetMetal Workbench - SheetMetal AddFoldWall
17	Pattern along a curve	Draft PathArray tool
18	Cut scope - cut tools affecting only selected part of the model	Different order of operations and use boolean cut on padded bodies
19	Merging adjacent faces	For faces of a PartDesign Body: change the Refine property of the last Feature to true, may not remove all the redundant faces For co-planar faces: use Draft Upgrade twice to get a Draft Wire, Draft Downgrade the wire to get a face
20	Hole tool using points from sketches	Draw circles for the Hole tool
21	Datum points from coordinates	Base datum points on existing geometry Create datum points at the origin and change their Position afterwards
22	A tool for automatic creation of ribs (structural reinforcements)	Create ribs manually, wedges (Part Wedge or PartDesign AdditiveWedge) can be used for simple triangular ribs
23	A tool for automatic creation of domes	Create domes manually, spheres (Part Sphere or PartDesign AdditiveSphere) with properly adjusted parameters can be used for simple spherical domes
24	Extending faces up to other faces (useful e.g. when extracting midsurfaces, as mentioned above)	Use the Draft Upgrade tool on the faces to be extended, extend proper edges with Draft Stretch and recreate the faces using Part MakeFace
25	Part Measure tool for radius or diameter measurement	Add-on Manipulator Workbench Add Draft Points to use for reference when dimensioning with Part Measure Linear or perform dimensioning in the Draft Workbench
26	Fuzzy versions of Part Boolean operations (possibility to specify a tolerance for boolean union and other operations)	Add-on Defeaturing Workbench
27	PartDesign AdditiveLoft and PartDesign AdditivePipe with a possibility to use an open profile as the first or last section	Different modeling approaches, e.g. involving PartDesign Pad
28	A tool to sweep a circular profile of a given diameter along a selected path	Draw the circular profile manually
29	Optional local coordinate system display for datum planes	Attach a datum coordinate system to datum plane to see its local orientation

Workarounds for the Draft Workbench

No.	Missing feature	Workarounds
1	Snap to apparent intersections of curved edges, perpendicular extensions, arc extensions, geometric centers and tangent points	Use the other available Draft Snap tools and a more manual approach with construction geometry When working on the XY plane: create a (temporary) projection of the geometry with Draft Shape2DView
2	Keyboard shortcuts for Draft Snap tools	Snaps can be activated and deactivated using keyboard shortcuts but only when none of the input boxes in the task panel has the focus (so the user should click in an empty space of the task panel to be able to use shortcuts for snaps)
3	Automatically change the colors of objects back to 'normal' when removing them from the construction geometry group	Move the objects to a layer with the correct color settings Change the colors manually
4	An option to quickly switch between the three main working planes and their projections at the selected point (for 3D drafting)	Set the Draft working plane to Automatic, and then select any of the standard views: front view, top view, etc. Use the Draft Constrain feature - snaps to axes, not to planes Use working plane proxies
5	Remove one arrow from a radial dimension	Add a line with an arrow: Create a Draft Line from the center of the arc or circle to a point on its edge Set the Arrow Type property of the line to "Arrow" and set End Arrow to "true" Create the radial dimension and snap to the endpoint of the line when defining its position Reduce the size of the arrows of the dimension to almost zero
6	AutoCAD-like command line input	Use FreeCAD's widgets or Python scripting for input
7	Hatch a region enclosed by wires	Create a face (a hatch can only be applied to objects with planar faces): In case of a single closed wire: set its Make Face property to "true", and its Display Mode to "Wireframe" Upgrade multiple wires two or three times until you have a face, or a single closed wire (see above) If the wires must stay separate, but are connected end-to-end, create a SubShapeBinder from them Trace over the region with a closed wire (not parametric)

Workarounds for the TechDraw Workbench

No.	Missing feature	Workarounds
1	Broken out and rotated/removed section views	Use the Slice apart tool to physically cut the model and then create its view
2	Auto diameter dimension on side views	Manually add the diameter symbol
3	Manually add geometry to generated views	Cosmetic line tools in Annotations and Extensions, limited Create regular views and Draft views of sketches and Draft objects
4	Shaded views in drawings	Place screenshots of the model on a white background on the TechDraw page
5	Ordinate dimensions	No known workaround
6	Broken (interrupted) views	Create broken views manually: Sketch two wavy or zig-zag lines close to the ends of a long part and extrude them towards the model creating surfaces for the cut Use the Part Slice tool to cut the model with these surfaces Hide the middle piece and move one of the remaining pieces towards the other Create a view of these objects If needed, make the lines of the cut dashed (using the TechDraw DecorateLine tool) If lines of the cut have to be extended, create a view of the sketch used in the first step and align it with the cut To obtain a proper value of the length of the cut part, you can either change the dimension value manually (after enabling the Arbitrary Text option) or link it to the distance between the end vertices of the original part
7	Exclude ribs from hatching	In some cases it might be sufficient to use the first workaround mentioned here and manually create a section with a custom cutting line
8	Export of TechDraw pages as PDF without making the text from the template (path text) unmarkable/unsearchable.	Export the page as SVG. Then convert the SVG to PDF by using e.g. Inkscape or open the SVG in a web browser and then save or print as PDF.
9	Box selection of TechDraw objects	Select objects manually, one by one (while holding Ctrl)
10	Modify regular and section views using sketching tools	Manually create and modify the views: If a section view has to be modified, use the Part SectionCut tool or boolean operations to cut the part in the same way as it would be done by the section view tool Use the Draft Shape2DView tool to create a 2D line representation of the view or section view Use the Drafting tools with proper snaps to modify the view Use the Draft Draft2Sketch tool to create a sketch out of the Draft objects Use the Sketcher ValidateSketch tool to make sure that the sketch has no missing coincidences, doubled lines and so on (those issues may impact the face selection in TechDraw) Use the TechDraw View tool to create a view of the sketch in TechDraw.
11	Auxiliary views	Create a standard view from the correct direction. Workarounds for "View normal to a face" may help. Rotate and position the view as needed.

Workarounds for the FEM Workbench

No.	Missing feature	Workarounds
1	Beams with arbitrary cross-section	Manually edit the input file and modify the beam section definition
2	Pressure load on shells, distributed load on beams	Force load
3	Support for multiple meshes and thus possibility to define contact between touching (not separated) faces	Apply Part Fuse or Part BooleanFragments to assemblies and include small gaps if you want to use contact or tie constraints
4	Apply torque to any surface	Transform constraint (only for cylindrical faces) Manually edit the input file - define a rigid body constraint and apply torque to its reference node
5	Define rigid bodies and virtual elements	Manually edit the input file and add proper keywords, use sets created by other features that can be deleted
6	Advanced material models (hyperelasticity, creep and so on)	Manually edit the input file and add proper keywords for material definition
7	Composite shells	Manually edit the input file and modify the shell section definition
8	Simple creation of node and element sets as well as surfaces	Use node and element sets and surfaces created by other features (material assignments, boundary conditions and so on)
9	CalculiX keyword editor that can fold data lines and allow changes not only right before running the analysis	Simple editor that can open the .inp file before running the analysis, color the syntax and save changes (accessed using the Edit .inp file button in FEM SolverControl window)
10	Meshing with hexahedral elements	Create the geometry in FreeCAD, export it for meshing in external software (e.g. Gmsh or Salome_Meca), import the mesh (e.g. in .inp or .unv format), drag it to the Analysis container and apply constraints to the geometry
11	Analyses with 2D (plane stress, plane strain, axisymmetric) elements	Prepare the geometry and analysis as if it were a shell model. Save the input file and open it with the built-in editor described above. Change the value of the TYPE parameter of the *ELEMENT keyword to the 2D element's name (e.g. CPS6 for plane stress) and replace *SHELL SECTION with *SOLID SECTION. Thickness is relevant for plane stress and plane strain elements. Save the input file and run calculations.
12	Multistep analyses (e.g. preload for frequency/buckling analysis)	Prepare the analysis with the first step, write the .inp file, edit it to add definitions of subsequent steps and run the analysis
13	Box selection of geometric entities for constraints	Select geometric entities manually, one by one

General workarounds

No.	Missing feature	Workarounds
1	Official assembly workbench	Three different add-on assembly workbenches
2	Improved appearance/rendering of 3D models	Link Branch Rendering in external software such as Blender
3	Status bar instructions (“Now pick this …”) for many tools that would benefit from them (e.g. Sketcher constraints), more informative tooltips	Wiki documentation
4	Consistent selection order - some tools require the user to pick the geometric entity first while others allow selection after enabling the tool	No known workaround
5	More GUI customization options - pie menus, different icon styles and themes and so on	Various customization packages created by the community Link Branch
6	Selection filter: picking only faces, edges, points and so on	Manual selection of proper geometric entities Wireframe mode to facilitate edge selection
7	Advanced selection tools: selection by angle, inverting selection, selecting inside faces and so on	Manual selection
8	Assembly workbench with an option to constrain parts to the origin and to datums	No known workaround
9	Transform tool with an option to move and rotate with respect to edges and global coordinates	Add-on Manipulator Workbench
10	More texturing options	No known workaround
11	View normal to a face (useful for creating specifically aligned views in TechDraw)	Select the face first when creating the TechDraw View. Macro Align View to Face In the Draft Workbench, select a face and press the Draft SelectPlane button. Deselect the face and press that button again to open the Working plane setup task panel. Click the Center view button. View normal to the face will be set. You can hide the grid and switch workbenches.
12	Highlight only the individual PartDesign feature in the 3D view when the corresponding operation is selected in the Tree view	No known workaround
13	Select only the individual PartDesign feature in the Tree view when a corresponding element is selected in the 3D view.	No known workaround
14	Freeform modeling	Model complex shapes in a "traditional" way - e.g. using add-on Curves and CurvedShapes workbenches Sculpt meshes, for example in Blender, and import them into FreeCAD
15	Assembly component generators and calculators for: bolted and riveted connections, shafts, splines, keys, cams, gears (spur, bevel, worm), bearings, springs, belts and chains, pins, o-rings	Fasteners Workbench and FCGear Workbench but no design calculations available PartDesign WizardShaft - basic calculations for shafts
16	A tool for kinematic analysis on properly constrained sketches	Python scripting - example
17	GD&T directly on 3D models - MBD approach	Draft Annotation tools