Making Linear Patterns Work in SOLIDWORKS

Today my challenge is to create a fixture to hold a part that has been machined using the lathe. It will be held in a tombstone mounting fixture for adding additional machined features.

The tombstone feature needs to be able to hold 4 of the turned items.

Here is the part that will be held in place.

Here I have created the cavity for the fixture.

When I look at this cavity in hidden lines visible style from the Top view, I can see there might be some problems with the fit in the areas highlighted:

Another way to analyze the interference is to use the Draft Analysis tool. Here the problem areas are indicated in red.

These areas will need to be trimmed away so the part will fit snuggly into the fixture. I will use an extruded cut to remove the negative draft shown above.

So, the next thing to do is to pattern this cavity across the fixture to create 3 more cavities.
I will open the Linear Pattern tool to perform this:

I have a good preview of the pattern I want, but when I complete the operation, I get this:

Clearly, I am missing something by trying to pattern the features highlighted above.

For my next try I’ll pick the faces. By using the face filter to volume select the faces, then selecting the vertical faces individually to add to the collection.

The preview looks good, but the pattern fails with this error:

The only option I have left is to pattern a body, but I don’t have a body to pattern right now. The solution is to create a body that can be patterned.
The technique I will use is “Intersect” to create a solid from the negative space.

First, I will need a plane or surface to make the cavity into a closed volume. By creating a new plane on the top surface of the tombstone feature I will be able to use it with the Intersect feature. I will also need to eliminate the fixture pin features at the top and bottom.

Next, I will use the “Intersect” Feature to create a solid from the cavity.

At this point completing the feature will give me two solid bodies. Now, I can use the linear pattern to create the three additional bodies.

Lastly, I will use the Intersect Feature again to remove the copies from the main body.

With a little cleanup of the extra solid bodies and the addition of a pattern of the fixture feature we now have a perfect tool for holding the parts.

I hope this blog has provided some enlightenment and more opportunities for using multi body techniques in your design strategy.

Thanks,

Dennis Barnes
Applications Engineer, Software Support
Computer Aided Technology, Inc.