Workarounds

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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, center points, 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 afterwards
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 Dimension diameter with respect to symmetry axis for revolved parts
  • Dimension radius instead (you can enter the diameter divided by 2 - the calculation will be handled by FreeCAD)

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, doesn't work for intersecting parts in assemblies
  • 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)
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)
  • Create ribs manually
23 A tool for automatic creation of domes
  • Create domes manually

Workarounds for the TechDraw Workbench

No. Missing feature Workarounds
1 Advanced section views (half, broken out, offset and aligned sections)
  • 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 Sketch in drawings
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.

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 was a shell model. Save the input file and open it with built-in editor described above. Change the value of the TYPE parameter of the *ELEMENT keyword to 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

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)
  • No known workaround
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 Assembly workbench with an option to constrain parts to the origin and to datums
  • No known workaround
8 Transform tool with an option to move and rotate with respect to edges and global coordinates
9 More texturing options
  • No known workaround
10 View normal to a face (useful for creating specifically aligned views in TechDraw)
  • 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.
11 Highlight only the individual PartDesign feature in the 3D view when the corresponding operation is selected in the Tree view
  • No known workaround
12 Select only the individual PartDesign feature in the Tree view when a corresponding element is selected in the 3D view.
  • No known workaround
13 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 importing them into FreeCAD
14 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
15 A tool for kinematic analysis on properly constrained sketches
16 GD&T directly on 3D models - MBD approach