From FreeCAD Documentation


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)
2 Chamfer tool
3 Circular pattern
4 Offset tool
5 Rotate tool
  • To rotate the whole sketch: change its Placement property
  • To rotate a selection inside the active sketch:
    1. Remove constraints that prevent the rotation, e.g. with Sketcher RemoveAxesAlignment
    2. Optionally add constraints between the objects to be rotated
    3. Apply an appropriate Sketcher ConstrainAngle constraint or drag a vertex of one of the objects
6 Scale tool
7 Adaptive dimension constraint
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)
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
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
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
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
2 Display the center of mass of the model (part or assembly)
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
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
7 Support for multiple solids within a body
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
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)
14 Guide rails for Additive Pipe and Additive Loft or their equivalents in the Part Workbench
15 Twist for PartDesign AdditivePipe or Part Sweep
16 Bending existing parts
17 Pattern along a curve
18 Cut scope - cut tools affecting only selected part of the model
19 Merging adjacent faces
20 Hole tool using points from sketches
  • Draw circles for the Hole tool
21 Datum points from coordinates
22 A tool for automatic creation of ribs (structural reinforcements)
23 A tool for automatic creation of domes
24 Extending faces up to other faces (useful e.g. when extracting midsurfaces, as mentioned above)
25 Part Measure tool for radius or diameter measurement
26 Fuzzy versions of Part Boolean operations (possibility to specify a tolerance for boolean union and other operations)
27 PartDesign AdditiveLoft and PartDesign AdditivePipe with a possibility to use an open profile as the first or last section
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

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)
5 Remove one arrow from a radial dimension
  • Add a line with an arrow:
    1. Create a Draft Line from the center of the arc or circle to a point on its edge
    2. Set the Arrow Type property of the line to "Arrow" and set End Arrow to "true"
    3. Create the radial dimension and snap to the endpoint of the line when defining its position
    4. Reduce the size of the arrows of the dimension to almost zero
6 AutoCAD-like command line 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
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:
    1. 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
    2. Use the Part Slice tool to cut the model with these surfaces
    3. Hide the middle piece and move one of the remaining pieces towards the other
    4. Create a view of these objects
    5. If needed, make the lines of the cut dashed (using the TechDraw DecorateLine tool)
    6. 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
    7. 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:
    1. 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
    2. Use the Draft Shape2DView tool to create a 2D line representation of the view or section view
    3. Use the Drafting tools with proper snaps to modify the view
    4. Use the Draft Draft2Sketch tool to create a sketch out of the Draft objects
    5. 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)
    6. 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
3 Support for multiple meshes and thus possibility to define contact between touching (not separated) faces
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
3 Status bar instructions (“Now pick this …”) for many tools that would benefit from them (e.g. Sketcher constraints), more informative tooltips
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
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
16 A tool for kinematic analysis on properly constrained sketches
17 GD&T directly on 3D models - MBD approach