I decided to do this project because a rival of mine casually remarked "why are you still using FreeCAD, it probably can't even follow the first tutorial of my browser-based CAD system?" The tutorial, which was apparently designed to show case the key features of his parametric CAD system, is based on a fully articulated mountain bike sub-assembly. I took the bet that if I could create essentially the same model in FreeCAD, he would buy the beer. Needless to say, he is eating his words and I'm drinking his beer!
I tried to follow the tutorial step-by-step using the Part Design workbench in as much as possible to get a good comparison. I am not able to share the FreeCAD file as I assume the design and dimensions in their tutorial are copyrighted, but several screens shots of the FreeCAD results are as follows:
- Articulated bicycle sub-assembly FreeCAD file. (The rear swing arm component is an imported .step file from the tutorial.)
- Picture1.jpg (284 KiB) Viewed 10307 times
The welded tube frame was a bit of a challenge but once the sweeps were completed, Part/Cutout for Objects worked quite nicely to create the intersection of each component. The intersection process was somewhat complex but presented no problems. Note that part of the upper bar is tapered which was handled by the PartDesign/Draft tool without any difficulty.
- Exploded view of the frame assembly showing the intersections required before welding.
- Picture2.jpg (260.38 KiB) Viewed 10307 times
One small feature that took me some time to figure out was a large radius around a notch in a thin-wall tube. I notched a solid tube first then applied the fillet followed by a pocket to hollow the tube. PartDesign fillet would not work properly around the notch for some unknown reason, but the Part/Variable radius fillet worked nicely if the start radius was 3 mm and the ending, 3.001 mm.
- Large fillet around a notch in the thin wall main upright tube
- Picture3.jpg (63.53 KiB) Viewed 10307 times
The billet rocker was perhaps the most difficult part to model since FreeCAD's Part/Thickness tool would not work on the 3D curved surfaces. A good work around was to use an extruded Draft/Facebinder to create the solid needed to Part/Boolean pocket the rocker body as in the tutorial. The other CAD system has a shell feature which can do it in one step.
- Sequence of steps required to pocket the relief in the rocker body
- Picture4.jpg (263.87 KiB) Viewed 10307 times
One feature used to demonstrate the articulated components was a fully constrained sketch driven by a spreadsheet. The only constraint variable required in the sketch is the ramp angle which can be changed in the spreadsheet. The components then had to be arranged manually using Placement properties and drone copies since the rocker is not entirely parametric due to the relief cutout.
- Sketch used for locating articulating components for an arbitrary ramp angle.
- Picture5.jpg (286.16 KiB) Viewed 10307 times
All-in-all this was a good exercise and demonstrated that FreeCAD V0.16 is already near world-class for most engineering tasks I encounter. Only a few features required workarounds and the only failures were the thickness tool and several overlapping fillets around areas that had to cross edges or those that disappeared at tangent terminations.
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
