Converting Detailed parts to be less detailed
Converting Detailed parts to be less detailed
(OP)
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
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






RE: Converting Detailed parts to be less detailed
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)
RE: Converting Detailed parts to be less detailed
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![[pc2] pc2](https://www.tipmaster.com/images/pc2.gif)
FAQ731-376: Eng-Tips.com Forum Policieswww.scottjbaugh.com
RE: Converting Detailed parts to be less detailed
Dan
www.eltronresearch.com
RE: Converting Detailed parts to be less detailed
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
RE: Converting Detailed parts to be less detailed
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
RE: Converting Detailed parts to be less detailed
-b
RE: Converting Detailed parts to be less detailed
Joe Dunfee
RE: Converting Detailed parts to be less detailed
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
RE: Converting Detailed parts to be less detailed
-b
RE: Converting Detailed parts to be less detailed
Eric
RE: Converting Detailed parts to be less detailed
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.
RE: Converting Detailed parts to be less detailed
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
RE: Converting Detailed parts to be less detailed
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.
RE: Converting Detailed parts to be less detailed
But, it is obviously a nice utility for simplifying solidworks objects.
Joe Dunfee
RE: Converting Detailed parts to be less detailed
RE: Converting Detailed parts to be less detailed
-Shaggy
RE: Converting Detailed parts to be less detailed
RE: Converting Detailed parts to be less detailed
-Shaggy
RE: Converting Detailed parts to be less detailed
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
RE: Converting Detailed parts to be less detailed
-Shaggy
RE: Converting Detailed parts to be less detailed
I did run a feature recognition on one of the connectors. It created about 80 features, and the file size swelled from 411k to 1,100k.
The simplify routine did recognize a number of small features, but in the end the part was still quite detailed because of all the external features.
In our case, I think the simplified version will be created manually (perhaps just a single rectangular extrusion). The mating needs to be done through the origin or default planes. I can't use this approach for any of our existing stuff, because it would involve re-doing all the mates.
Since we include every pin that is used in each connector (some pins are omitted in some situations), we also need to simplify the process of doing the mates. Obviously the answer is to create smart mates.
This overall project has been several years in development, and now is nearing completion. It is the first project they've done using Solidworks. I think there is always a lot of stuff you wish you did differently when it is the first time through an entire project. The next project should be much smoother. I will recommend that we not reuse any of the parts from the current project.
Joe Dunfee