Saturday, September 22, 2012

New Part Design features

Recent FreeCAD (see info at the bottom) introduces new Part Design features.

The updated Part Design toolbar, from the left side:
  • Create a sketch
  • Close the sketch
  • Pad
  • Pocket
  • Revolution
  • Groove
  • Fillet
  • Chamfer
  • Mirror
  • Linear pattern
  • Polar pattern
  • Multitransform (mirror, linear/polar pattern combined)

New functions - basics

Create an rectangle (sketch) on the XY plane. The rectangle should be symmetrical to X and Y axes (simply select two corners and an axis then click symmetrical constraint button).

Pad the sketch. Please notice new available options: type (Dimension, To last, To first, Up to face, Two dimensions) symmetrical (yes/no),  reversed (yes/no).

Select side face on the pad, and sketch a rectangle. It will be used for a groove feature. The groove is similar to pocket but material is removed around axis (like in a revolution).

Select the sketch and click Groove a selected sketch. Adjust angle and side in the Tasks tab. Note: sketches for almost all features (except pads) need a support face. The face should be selected before you start sketching - in other case use Map sketch to face from Part Design menu.

In next steps you will create a mirrored feature. Select the top face and sketch a circle.

Pocket the circle, set pocket type to Through all.

Select the pocket and use Create a mirrored feature. Set plane to XZ. Note: mirror of multiple holes can be unsupported in actual version of FreeCAD (implementation needed).

Linear pattern is an another useful function. Create a pad on side face, parallel to XZ plane.

Select the pad and use Create a linear pattern feature. Set direction to X, adjust length (should be lower than the body length) and occurrences number.

The most advances is a multitransform feature. You can mix linear and polar patterns and mirrored or scaled features. Select top face.

Sketch a circle close to (0,0) point.

Pad the circle.

Use Create a multitransform feature. Right click in the Transformations text area and then Add linear pattern.

Set occurrences to 2 and direction to X.

Then you can Add polar pattern in similar way. The direction is Z and occurrences is 5 (experiment with them!).

I want add XY mirror but in this case body must be symmetrical to XY. Edit the first pad - set Type to Symmetric to plane.

Now you can finish edit the multitransform feature. Use right click to Add mirrored transformation. Set plane to XY.

The final effect:

Download file.

Download RAW Video.

FreeCAD version:
Version: 0.13.1486 (Git)
Branch: master
Hash: aaaa7eb30313e25614b7f1b95b544788d8fa99fc


  1. Great update, useful tools

  2. I am very curious about the Pattern feature: when you are done creating the pattern, can you break the parts created by Pattern apart? I'm working on a PolarPattern that creates 8 cubes around a 360 degree circle, but then I need to rotate each cube at its own angle around an axis that goes through the center of the cube, i.e. it's different axis of rotation for each cube. So, I really need to treat these cubes as separate parts, but PolarPattern appears to be one monolithic part, sort of like a gear with those 8 cubes as the teeth of the gear and I don't seem to find any way to break them apart. Any clues?

    I'm going to see how I can post a picture to illustrate what I'm asking about, see below. Oh, and it's version 0.13 1830(Git) 64-bit Linux. Thanks!

  3. Thanks! I ended up using multiple copies of the cube Part (created as a cube, not as a pattern from sketch) and I did not actually need all 8 copies because they were all supposed to be use to "carve" a piece of the cone at a particular angle, so I just rotated the cone each time I needed to make a cut in it.

    The attached picture shows how the almost complete part (the cone with sides shaved off 8 times) and the last, 8th cube just about to make the last cut in the cone look like.

    Thanks again for the tutorial, I'll be sure to use patterns as you describe next time.