Impossible Models: Manufacturing Concerns – Shelling

My storage of customer files has 280 folders. Generally that’s one or more projects per customer, and some have a lot of projects in each folder, and most projects are multiple parts. When I think back and try to identify some of the most challenging parts from a manufacturing point of view, it can be tough. Most of the parts I’ve done have been plastics, and plastics are a good source of tough modeling situations. I rarely go as far as splitting cavity and core, but the parts have to be correct from a molding point of view.

Draft is very often tough. It is sometimes something you can’t just add on as a “draft” feature. You have to actually model it, feature by feature, and sometimes face by face when the draft has to be surface modeled. But I’ll talk about draft another time. For this article, I want to talk about Shelling.

There are a couple parts I want to look at where the shelling could not be done using traditional methods. In some cases, the parts are deceptively simple, and you’d thing “oh, this is a straight forward plastic part”, and you’d be really wrong.

Here’s a part that was harder than it looks. It doesn’t have any swoops, no surfacing features, it looks like extrudes and cuts. It was a custom manifold that the customer wanted to mass produce by injection mold. It included valve bodies, meter connections, seals, mounting bosses, brass threaded inserts, and so on. And it had to be shelled for injection molding.

Since many of the holes are transverse, we had to reconfigure the manifold so that it could be molded with side action pins. These pins can’t penetrate one another, so the function of the actual manifold and valves had to be planned according to the rules of injection molding. It took a lot of back and forth just to get the layout right.

The tough part from the modeling point of view was shelling the part, and filling in the occluded areas. I don’t remember the reason, but the Shell feature would not work on this part. It was an error I hadn’t seen before, and haven’t seen since. I think there were too many interior bodies created by the shell feature. It had to be shelled manually. You can only imagine what that would mean on a part that looks like this.

I can’t walk you through all the attempts that I made in shelling this part, but the final process looked something like this:

• model manifold as if it were to be machined from a block of brass
• copy a block of material over the manifold
• subtract the actual manifold from the copy (this gives a solid model of the interior space of the manifold)
• create a simple shell of the outside of the part (outline of the part extruded and shelled)
• use the interior space (in chunks) with the Indent feature to add shelled areas to simple outside shell
• Use the Undercut Detection tool to find occluded areas, and fill them with regular extrude features (add draft)

The trick here was really the Indent feature. The highlighted areas below were the geometry created by Indent. The dark green was the simple outside shell. The blue, yellow and green were interior cavities that I had not yet used to Indent at this point in the model.

This turned out to be a massive multi-body exercise, as well as learning about the limits of the Indent feature.

Let’s look at Indent, since most of you probably haven’t seen it.

Take a thin plate, and put some bodies on it, flush with the surface, not merged, and intersecting with the plate material. It should look like this:

Now start the Indent tool (Insert/Features/Indent).

The Target body is the plate. The tool body regions area the red and yellow bodies below the plate. Use the Keep Selections option. The Thickness parameter can be set to anything, but ideally the thickness of the plate. The field under the thickness is the clearance, so you can make a gap between parts and a housing. You can see the clearance in the image below.

The finished part looks like this (with the tool bodies removed):

So you can see how the Indent feature can be used like a shell, and how the use of multiple bodies makes that very useful.

Anyway, that’s how this part was done. It looks simple enough, but with the Shell error, it quickly became very complex, and an big exercise in creative problem solving.

Here was another one.

This part had to be shelled. But guess what? The shell feature wouldn’t work again. I’m sure I went through all sorts of contortions to try to get the shell feature to work, but it just wouldn’t go. Again, all of this work was probably 7 years ago.

When you come up against stuff like this, people suggest a lot of creative stuff that in the end doesn’t work conceptually. Like Scale. There is nothing you can do with the Scale feature to shell out this part. You need to offset a specific distance, not scale by a percentage. Oh, and by the way, offset won’t work either, probably for the same reason that Shell won’t work.

Actually, the solution to this one was simpler than most.

In this case, I offset the outer edge (I may have had to approximate some things with hand sketches, because you know this kind of thing doesn’t always work automatically) and created a cut using Offset From Surface, using the outer faces as a surface body. It worked. It wasn’t really, technically 100% conceptually what it was supposed to be, but it was close enough. We just needed to hog out material from the back so that the casting wouldn’t deform as it cooled. Plus, who needs 15 pounds of brass when 3 will do?