PartDesign Bearingholder Tutorial II



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 fillets. 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 second part of the tutorial. It will use what might be called the 'multiple 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 which has an inside diameter of 40mm). 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
Create a new part in the PartDesign workbench. Rename the Body that is created by default to Skeleton. This Body is probably activated already, which you can see by the blue background colour in the feature tree. Create a new sketch on the YZ plane containing the outline of the shaft, bearing and sealing rings. After finishing the sketch, make a revolution feature from it. This skeleton feature will later be used to reference the real geometry to it. This means that if you want to change any dimensions, all you need to do is adjust the skeleton feature's dimensions and the rest of the part will update accordingly.

The main body
Create a new body and make it active. The sketch for the first pad is shown on the right. It is placed on a datum plane with an offset of 5mm (wall thickness) from the skeleton face marking the side of one of the bearing sealing rings. Because all the important dimensions are taken from the skeleton, there are just three dimensions: The machining allowance (3mm) at the base as an offset to the XY-plane, the 5mm wall thickness from the outer diameter of the skeleton, and the two degrees draft angle. Two create the 5mm dimension, you first need to select the outer circle (radius 45mm) of the skeleton geometry as external geometry in the sketcher, and then put in a construction line constrained tangential to this circle and at an angle of two degrees.

You are probably wondering why there is this 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), create a Pad from it extending up to the other side of the skeleton geometry, again with a 5mm offset to the side face. You don't need to create a datum plane this time, the "up to face" mode of the Pad dialog offers to input an offset.

Next, we will cut away some material on both ends of the Pad because it is always ideal for cast parts to have as uniform a wall thickness as possible. Create a sketch on each of the end faces of the Pad and dimension it at 5mm offset from the circle representing the bearing sealing ring (radius 27.5mm on one side and 34mm on the other). For the bottom line segment of the sketch, create another external geometry from the Pad and constrain to this. Thus the sketch has only a single dimension, the 5mm wall thickness (the 150mm and 75mm dimensions are not important as long as they are large enough to ensure that everything is cut away).

Use the sketch you created to make a Pocket and extend it to the face of the skeleton geometry that represents the bearing, minus 5mm offset for the wall thickness. For the second Pocket, you can use the option "Duplicate selected object" from the Edit menu to duplicate the sketch you already made (choose not to duplicate dependend objects if the question pops up). Then, select the face you want to move this sketch to, and tell FreeCAD to map the sketch to this face (this is an item on the PartDesign menu). After creating the second Pocket, you can look at the result from the bottom to check that you have a uniform wall thickness of 5mm around the contour of the skeleton geometry.

Now it's time to create draft and fillets. The draft feature requires a neutral plane, meaning that the geometry that is cut by this plane will remain in its place, while the rest of the face is tilted at the draft angle. Using the bottom of the Pad for this purpose for this is not a good idea, because the wall thickness in the top part of the holder would become less than 5mm. So we create a datum plane offset about 35mm from the XY for this purpose. Activate the Skeleton body and create the plane there, because we will need it for applying draft to other bodies, too.

The picture on the right shows the finished first body with draft and fillets applied. Note that the outer (concave) edges have a larger fillet radius of 5mm, again with the purpose of creating a more uniform wall thickness (more than 5mm is not possible because then after machining the inside of the holder the wall thickness would become less than 5mm).

Hollowing out the main body
We will now work on the inside of the holder and hollow it out to make space for the bearing and sealing rings. When doing this of course we need to keep in mind the 3mm machining allowance. Since this tutorial teaches the multi-body method, we will create the inside geometry as a separate body and then cut it out of the main body with a boolean operation.

Create a new body and make it active. First, we need a datum plane offset 3mm inside the skeleton face that shows the side of the bearing. Then, duplicate the sketch of the first Pad of the main body. It will be added to the main body, so right-click on it and choose to move it to the newly created body (this option is only available in the context menu if the PartDesign workbench is active). Map the sketch onto the datum plane (if the sketch turns upside-down after mapping, move the datum plane to the other side of the bearing, next to where the duplicated sketch is located). Now, modify the sketch so that the diameter is 3mm less than the outer diameter of the skeleton geometry that represents the bearing. All you need to do is remove the 5mm dimension, drag the sketch inside the reference circle, and create a new 3mm dimension.

Next we want two more Pads to hollow out the place for the sealing rings. Duplicate the sketch of the first pad of the cut-out Body and map it to the XZ-plane. Edit the sketch and replace the external reference with the outer diameter of the bearing sealing ring. Extrude this sketch to an offset of 3mm of the side of the sealing ring. Repeat the whole process for the sealing ring on the other side.

After this we want to create two more Pads like the last two to give the shaft a clearance (e.g. 3mm) inside the holder.

Now all that remains is to apply draft to the planar side faces, using the same neutral plane as for the main body, and filleting. Apply a general fillet of 3mm to all edges. You will notice that there are several edges that cannot be filleted... this is a defect of the underlying geometric kernel which FreeCAD uses.

We are ready to hollow out the main body. Select it and choose to create a new Boolean operation. Add the cut-out body to the list window and set the operation to "Cut". The result should look like the picture on the right.