PartDesign Bearingholder Tutorial I



This is an introductory tutorial to modeling with the PartDesign workbench in FreeCAD. The purposes of the tutorial are to introduce you to two different workflows for creating a cast part with drafts and rounds. Depending on what other CAD programs you have been using, one or the other might be familiar to you. As a working example we will be modeling a simple bearing holder.

This is the first part of the tutorial. It will use what might be called the 'single body' workflow, using the (simpler) top part of the holder as an example.

Obviously, to follow through this tutorial you must activate the PartDesign workbench.

Design data
The holder should be able to hold a diameter 90mm bearing with a width of up to 33mm (e.g. DIN 630 type 2308). The bearing requires a shoulder height of at least 4.5mm in the holder (and on the shaft). The top part of the holder will be bolted to the bottom with two 12mm bolts. There should be a groove on both sides of the bearing able to hold a standard shaft sealing ring DIN 3760: 38x55x7 or 40x55x7 on one side, 50x68x8 on the other side.

The holder will be a sand cast with a minimum wall thickness of 5mm, a draft angle of 2 degrees, and a minimum fillet radius of 3mm.

Setting up the skeleton geometry


The idea of skeleton geometry is to capture the basic design dimensions in a single datum feature (e.g. a plane or an axis). When the design dimension changes, all that needs to be done is to change the skeleton feature. If the model is well built, then all its feature will recompute to reflect the design change. This reduces the danger that in a complex model, where the basic design dimensions are used in multiple places, you forget to change it somewhere.

The alternative to skeleton geometry is to have a table of the basic design dimensions that assign a symbolic name to each dimension, and then use the symbolic name wherever the dimensions is required to build the model. FreeCAD does not allow this approach yet.



For the case of the bearing holder, the two most important design dimensions are the distance between the bolts (which limits the size of the bearing that can be used) and the height of the bolt heads. The dimensions chosen are
 * Distance between bolts: Radius of bearing (45) + wall thickness (5) plus radius of hole for bolt (7) = 57mm, so the vertical plane will be 57mm offset from the YZ-plane. To create this datum plane, select the YZ-plane and then choose to create a new datum plane. Enter the offset in the dialog that opens up
 * Height of bolt heads: This was chosen as an offset of 28mm from the XZ-plane

For convenience, two further datum planes can be created to reflect the amount of material that must be cut away from the sides of the bearing holder. They are offset +22 and -22 from the XY-plane.

It is advisable to give clear names to the skeleton geometry. Most of the time, you will want to turn off visibility for datum planes because they clutter up the screen, and if the planes have self-explanatory names you can just pick them by name instead of from the screen.

The actual solid geometry


Now its time to start creating some real geometry. The sketch for the first pad is shown on the right. It is placed on the XY-plane. There are just three dimensions: The inner radius (22.5mm), the machining allowance (3mm) at the base as an offset to the XZ-plane and the distance from the datum plane representing the bolt axis (7mm). This means that if you later move the datum plane, the pad will automatically adjust its outer radius. You are probably wondering why there is a small straight segment at the bottom of each arc. This segment ensures that there will be a draft angle of 2 degrees on the arcs. This might look like a lot of work for a very small benefit, but many CAD programs (and maybe FreeCAD one day) have tools that highlight a solid model in different colours and immediately show you all faces where the draft angle is not correct. Yu don't want that to happen to your model, especially after putting on a lot of fillets!