TechDraw Pitch Circle Tutorial

From FreeCAD Documentation
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Time to complete
10 minutes
FreeCAD version
Example files
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This tutorial explains how to add a pitch circle to a TechDraw view. It assumes that the model is a PartDesign Body with at least three holes in a circular pattern. For the circle a separate sketch will be created. A similar procedure can be used in other situations and to add other annotation-like elements to TechDraw views.

In FreeCAD version 0.20 and above a pitch circle can be created with the TechDraw ExtensionHoleCircle tool.

Create the sketch for the circle

  1. Activate the PartDesign Body. This will also activate the PartDesign Workbench, if required.
  2. In the 3D view select the correct face belonging to the body.
  3. Create a new sketch with the PartDesign NewSketch command.
  4. The sketch will be attached to the selected face.
  5. Call the Sketcher External command.
  6. Select three circular edges (holes) from the body.
  7. Use the Sketcher Create3PointCircle command to create a circle constrained to the center points of the external geometry.
  8. The sketch should now be fully constrained.
  9. Close the sketch.

Create the TechDraw view

  1. Switch to the TechDraw Workbench.
  2. If you don't have one already: create a TechDraw page.
  3. Make sure the 3D view is properly aligned.
  4. Hold down the Ctrl key and in the Tree view select the body and the sketch that was just just created.
  5. Insert a new view by calling the TechDraw View command.
  6. Switch to the TechDraw page.
  7. Select the circle.
  8. Call the TechDraw DecorateLine command.
  9. Change the Style and Weight of the circle.