Converting Detailed parts to be less detailed

[cadcoke5]

We use a lot of connectors from Tyco electronics. Tyco has very detailed 3-d models of their connectors online, and this is what we use for our circuit board assemblies.

However, their models have every tiny internal detail... far more than what is needed for our uses. I expect they are causing performance issues with our main assembly.

The connectors are already imported and saved as a multi-body part. I suppose the circuit board assembly itself could be converted to a multi-body part. But, I am looking for general suggestions for how others deal with this issue.

I imagine that I can create two configurations in each connector part. One is the version I imported from their web page, and the other being a very simplified version that I model myself. But, then I would want an automatic way to switch between the versions on the main assembly.

Also, I recall hearing the term "shrink wrap". This refered to a software feature to take a complex assembly and only show the outer skin. If I recall correctly, it would also automatically plug holes below a certain size. This sounds like a great automatic way to simplify my connector models.

I know an assembly can be exported as "external faces" when converting it to a multibody part. But if it already a part, then this option is not available. Also, it doesn't have any features to plug small holes.

Is something like the "Shrink Wrap" featured available for SolidWorks?

---
Joe Dunfee

 

[CorBlimeyLimey]

I believe "Shrink Wrap" is a Pro/E or UG term.

If the part has features and/or multi-bodies, you could just suppress or delete the offending details/bodies.

If it doesn't have features you can you create them using Feature Recognition ... and then suppress or delete them.

If you don't have Feature Recognition, you may have to adjust the model manually using various functions. (Cuts, Extrudes, Deleting faces, etc)

 

[SBaugh]

In the assembly, you can save more the outer external faces... that just makes surfaces and creates more performance issues. You can also save out as "External components" and that saves out only the parts you see outside.

As for parts there is nothing that will compress the file itself down from a SW standpoint, but you could save out as Parasolid. You lose the FM tree and the parasolid functionality like you initially had. But it does compress the file down.

Shut off surfaces are used in conjunction with Tooling splits, but that is the only thing besides a surface to shut off holes, unless you just extruded over the holes. Then it would merge the bodies into a single body.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[Eltron]

You can also load the components lightweight in your assembly.

Dan

http://www.eltronresearch.com

 

[ShaggyPE]

Create a second configuration in the connector part file (call it SIMPLIFIED etc). In this second configuration, add a couple of features that fill in the detail of the connector. Be sure to leave the features that will be used to mate it to the board. In your board assembly, add another config called SIMPLIFIED also. You can now have two configs, one detailed and one simplified. Use the simplified config on the next assy up.

Even though there are more features in the simplified part configuration, this will result in a more manageable part because of the lack of detail.

-Shaggy

 

[cadcoke5]

Actually, my part has a lot external detail, so the "save surface" method won't help much. It is becoming obvious that I must manually model the simplified version.

I will create two configurations of the part. One will be called "Detailed" and the other "Simplified". However, I still am puzzled about how best to switch between the two in my higher level assemblies.

I realize I can create my sub-assemblies with the two separate configuration that refer to the two separate part configurations. But, since I have multiple levels, this may get cumbersome. I think I need a way to automatically switch just the parts between the two configurations while I am in a top level assembly.

Hmmm... I am not sure the above will work. Perhaps configurations are not the way to go. Perhaps the bodies that represent the detailed part have the word "Detailed" on each of the bodies. Then, my detailed features have the word "Simplified" in the name of the feature. A VBA macro would be needed to search through all sub-assemblies and suppress/unsuppress the correct features.

I've done VBA programming for AutoCAD, but haven't done it in SolidWorks yet. Does the above paragraph sound viable?

Joe Dunfee

 

[bvanhiel]

Just create a "detailed" config at the top level assy. Seems way simpler than writing a VBA script.

-b

 

[cadcoke5]

But how do I get all my sub-components and sub-assemblies to be set to show the correct level of detail? I imagine you are expecting me to manually do it. Right?

Joe Dunfee

 

[ShaggyPE]

But, since I have multiple levels, this may get cumbersome. I think I need a way to automatically switch just the parts between the two configurations while I am in a top level assembly.[quote/]

This is where design tables come in. With well named configurations, you can generate your simplified assembly configuration within the design table.

As far as using configs, they are much easier to control than using separate parts whose suppression states are on/off. Also, you will have far fewer mates when using configs (as long as the faces exist in both configs).

-Shaggy

 

[bvanhiel]

You don't need design tables. The top level "detailed" config will reference the sub-assy "detailed" configs. The sub-assy "detailed" config then references the "detailed" config of the parts. The top level "simple" config references the sub-assy "simple" config and so on.

-b

 

[EEnd]

If you feel like writing a VBA script, you could make one that drills down through an assembly and its subassemblies making detailed and simplified configurations of any assembly which had one or more components which had their own detailed and simplified configurations. I think something like that would save quite a bit of effort in setting up (and potentially maintaining) the configurations.

Eric

 

[CorBlimeyLimey]

cadcoke4 ...

If you have the Utilities add-in, you may be able to use the Simplify function.
Enter Simplify part in the Help file index.

 

[cadcoke5]

Thank you very much. The Simplify Part function is what I was looking for. The see the Search feature of the utilities is also a good feature for my purposes. It will allow me to search for stuff like small holes or fasteners and then suppress them all at once.

The phrase "simplify part" was not in the main help files, so my search efforts there didn't turn up anything. I had to install the utilites and search their help file.

Joe Dunfee

 

[CorBlimeyLimey]

You're welcome.

Let us know how well it works. I only have the basic SolidWorks version so I've never had the chance to use it, or even see a demo of it.

 

[cadcoke5]

It looks like a no-go for me. The imported parts are just solid bodies... no features. The simplify utility will only search for Solidworks features on objects (such as holes, cuts and fillets)

But, it is obviously a nice utility for simplifying solidworks objects.

Joe Dunfee

 

[CorBlimeyLimey]

Run the part(s) through the Feature Recognition module first. That will give you the features for suppression by Simplify.

 

[ShaggyPE]

I still think your best bet is my suggestion above.

-Shaggy

 

[CorBlimeyLimey]

Shaggy ... I agree, DTs are the best way to control the configs, but they can't simplify the actual parts to be used in the configs.

 

[ShaggyPE]

He would add a few features to the parts that would not generate new faces. These features would "fill" in the detail that is on the part. Picture taking a super detailed board mounted connector and adding a couple of features to turn it into a solid block. Making sure not to lose the surfaces that are used to mate in the next assembly. This would allow him to switch configs in the assembly and not screw up any mates. The DT is only used in the assembly to quickly generate the simplified config. He can change all part configs to simple in one swoop.

-Shaggy

 

[cadcoke5]

Picture taking a super detailed board mounted connector and adding a couple of features to turn it into a solid block. Making sure not to lose the surfaces that are used to mate in the next assembly.

I didn't think of this issue. That may actually be a very big issue. I can make a solid that will fill in some holes, but external protrusions are another thing. Perhaps that will just be a limitation of this method.

Joe Dunfee