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Both methods will work and both have pros and cons, depending on your preference and situation. You can pull the overmold body out of the multi-body part by RMB on that body in the Solid Bodies folder and clicking insert into new part. The references will be maintained, and you won't have an assembly file but you will have the 2 part files you desire. I would probably use this method, but there is something to be said for the ease of manipulating parts via mates in an assembly.
My methodology is pretty simple. If it gets two part numbers, it is two different parts (either Matt's suggestion above, or as two parts in an assembly). If it is one part number, then it is one part with multiple bodies (double shot injection molding, purchased as a single item, etc).
As for how it is modeled and SW's capability, you might get a bit more control by not using an assembly, and using some sort of multi-body part. Mainly, if you make significant changes to the model later, it will be easier to update a multi-body part; while if they are different parts in an assembly, you will probably lose all references and have to do a lot of re-creation to the overmold.
Our approach is similar to Charles's. If the drawing includes a BOM, then we create the component files and an assembly file. If there's no BOM, we will try to use solid bodies. For an overmold, we would not have a BOM and would use solid bodies.
It seems the SolidWorks help tutorial suggests three possible methods: multibody, base part, or split part. I have not yet decided which approach to use for an overmold.
The following information is found in the SolidWorks 2007 tutorial:
Why Use These Techniques Instead of an Assembly?
' SolidWorks strongly recommends these techniques instead of an in-context assembly for these reasons:
Performance. With an in-context assembly, it would take 10 times longer or more to rebuild because every change made in every part requires a complete rebuild of every part, whether it has a change at the part level or not.
Design Intent and Best Practice for Design. The three techniques follow a clearly-established master part methodology in which the master part captures the design intent of the shape and propagates this intent to its injection molded components. These techniques work well because they use a one-way driven process where the master part always drives the derived parts.
In an assembly, the design process is different. In fact, the advantage of in-context assembly design is that you can choose multiple situations between the parts in the assembly, where parts drive or are driven.'
I always do these as single part files using multi bodies, then save the bodies out to an assembly file. Often you need to supply tooling with the two parts depending on the way it is tooled. This way you have a master model single part file and children individual parts and assemblies all linking back. Never really had any huge issues with this and SW2009 is even more robust.
As for the surface texture for the grip its down to your design really. If doing dimples I tend to create a sphere body slightly above (for recesses) or below (for raised) the surface to allow for draft, then either pattern these bodies or manually place them on the surface, then Combine Add or Subtract them to the main body. Sometimes it can get a bit tedious! A knurl pattern there are many ways to do this as a feature depending on the geometry of the surface it is getting placed onto.
From the suggestions I have received, it seems the majority favor a multi-body approach for creating an overmold. I did receive a suggestion about using the indent tool, but I am concerned about model stability if the design intent is changed in the future. Also, is the indent feature practical for a production model part?
Parel Design has a blog link to a very useful tutorial called SolidWorks Overmold Technique.
' Today I will share a really cool method for designing overmold. I had been using a pretty intense method of offseting surfaces in and out and knitting them together with a bridging surface (most likely a trimmed surface extrude) This method is a little more stable because it relies on more Solid features, which tend to have less problems with relationships.'
Before I try the multi-body approach, I am awaiting the hand-sketch concepts from an industrial designer I consulted with for a second opinion. I have done a few overmold designs in the past using Pro/Engineer, and wanted to know the best approach / technique in SolidWorks. I had fully designed the parts recently, and now that an overmold design needs to be incorporated into the parts, the model stability and rebuild performance are of major concern.
What i've done in the past was create a multibody part and then save the bodies as part models.
Like Charles, we'd have a part number for the plastic and a part number for the overmold, so it needs to be 2 part files.
I keep all the external ref. incase there are changes down the road.
Has anyone used the indent feature for creating overmolds? This tutorial titled Using Indent to form a handle describes the process of creating an overmolded handle.
On the surface, this method of creating an overmold seems the least cumbersome of the techniques I have reviewed to date. Is there any reason not to use this method in favor of other overmold creation techniques? I do not see a problem with creating mold tooling from the part models.
I thought the overmold technique from Parel Design (from my last post) was very informative as well. Before I start creating models using the indent feature, I would like to know if I should be aware of any potential problems with using this technique such as model stability. The area for the overmold will have bosses and ribs (opposite wall surface of the overmold) after the shell feature has been created.
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We haven't used the Indent tool for overmolded parts. I'll have to look into it. When Indent first came out, it was not very robust, so we gave up on it pretty quickly.
We usually make overmolded parts as a multi-body part and then save the bodies into an assembly. One reason to save them out as separate parts is if your materials have significantly different densities.
Very often I work in multybody it very conveniently.