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 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. Remember that before you can use the datum plane for dimensioning, you need to introduce it as external geometry to the sketcher.

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. You don't want that to happen to your model, especially after putting on a lot of fillets!

When you have done the sketch (which is a bit tricky because of the 2 degree tangential lines), just pad it symmetrically to the sketch plane with a length of 62mm: 34mm for the bearing, 2x 9mm for the sealing rings, 2x 5mm for the wall thickness.

Next we want to cut away some material where the sealing rings are, because their outer diameter is much less than the bearing's. The easiest way to create the sketches is to select the sketch of the pad and then choose "Duplicate selection" from the edit menu. You can then remap the sketch to the side of the pad, and modify it as shown in the picture.

The only two important dimensions in the sketch are 3mm of machining allowance at the bottom, and a inner diameter of 78mm: 68mm for the outer diameter of the sealing ring + 2x 5mm wall thickness. Since the sealing ring on the other side will only have a diameter of 55mm, the cut-out can be 65mm here.

After you have created the sketch, pocket it up to the datum plane marking the bearing side plus 5mm wall thickness. If you ever want to modify the holder to be able to hold wider bearings, all you have to do is to change the dimension of these datum planes, and the cut-out depth will follow along.

To reduce the amount of machining required, we also want to cut away some material inside the holder. Again, duplicating the sketch of the first pad is convenient. It doesn't even have to be remapped. Again, the only important dimensions are the machining allowance (3mm) and the outer diameters: 84mm for the place where the bearing will be (90mm - 2x machining allowance), 49mm for the smaller sealing ring (55mm - 2x 3mm) and 62mm for the larger sealing ring.

After creating the sketches, pocket them: Symetrically 28mm for the bearing cut-out (34mm - 2x machining allowance) and one-sided 23mm for the cut-outs for the sealing rings: 34mm / 2 for half the bearing width + 9mm for the sealing rings - 3mm machining allowance.

Your part should now look like the picture on the right. Note how the different cut-aways combine to create an almost uniform wall thickness, which will make the casting easier and less liable to have pores.

Now all that remains is to create some material for the bolts to go through. You might be tempted to sketch these as a circle and then pad them, but this will head you for trouble when you try to put the draft onto them later (I assume that is a weakness of OpenCascade). So to circumvent the problems, it is better to create a sketch with the draft angle included and then rotate it through 360 degrees.

Here again the skeleton planes come in useful. You will need the bolt axis plane and the bolt head plane as external geometry. Then, create a straight line for the rotation axis and make sure it is constrained to the bolt axis plane reference. Toggle it to be construction geometry. Then, sketch the rest of the contour. The important dimensions are the machining allowance at the top and bottom and the radius of 12mm: 7mm for the hole radius + 5mm wall thickness.

Create a revolution feature from the sketch and then mirror it on the YZ-plane. This is all the solid geometry we need to model. The rest is draft and fillets.