Tuesday, September 25, 2012

"Part" Mirror vs "Part Design" Mirror

Some tools (Mirror, Chamfer, Fillet) seem duplicated in Part and Part Design Workbenches. Despite names, they work in slightly different ways. Part is designed for low-level operations on solids, Part Design is for higher level operations on features.

Part workbench Mirror

Start a new sketch. Draw a square or rectangle on XY plane and create a pad. The rectangle should be symmetric to axes. 

Make a pocket on a side face.

Open Part workbench, use the mirror (Mirroring a selected shape) tool and select a plane (YZ or XZ) in Tasks tab.

Confirm operation, now you should see second, mirrored solid. You can hide Pocket or Pocket (Mirror #1) with [Space]. 

Part Design workbench Mirror

Delete or hide Pocket (Mirror #1) and back to Part Design workbench. Select Pocket and use the mirror (Create a mirrored feature) tool. Set the plane to YZ (or XZ). As you can see, Part Design mirror works different. The pocket feature is mirrored instead the solid object.

Version: 0.13.1489 (Git)
Branch: master
Hash: a20f4dddffbe590434041373ee125b367ee60e31

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

Tuesday, September 18, 2012

First FreeCAD book has been published

FreeCAD: Solid Modeling with the Power of Python (authors: Daniel Falck, Brad Collette) has been published. 70 pages, English. More info: