Looking for tips on using toolbox, smart fasteners with PLM system.

We need to modify SolidWorks Toolbox fasteners in such a way as to:

  1. Have a single unchanging part (such as socket head cap screw) that can be placed into our PLM as a "read only part" covering all our company's standard sizes for that type of fastener. (Currently our trouble is that we see configurations being added on the fly)
  2. Have the fasteners work correctly with Smart Fasteners, and also with the fastener toolbox.
  3. Have our company's standard part numbers and descriptions show up correctly on the BOM.
  4. Have the SolidWorks design tree show a reasonable name and description for the part (currently we see a number like: B18.3.1M - 2 x 0.4 x 4 Hex SHCS -- 4NHX-V1 where we want to see our part number and description)

Also, How should I make standard assemblies (like air cylinders) where the designer may want to add configurations specific to his application. I do not want to have to store every configuration as a seperate part, or have to rev the cylinder assembly every time we add another configuration.



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What is the PLM product? There are different ways of handling this. Some software will put a placeholder in the PLM and keep the file outside it.

Getting rid of the adding configs on the fly is definitely a best practice for Toolbox. There are various ways of doing that, including pre-building all the configs and using individual part files instead of configs. It sounds like you want to use configs, and don't want individual parts, so you will need to pre-build each size fastener your company will use.

To do this, you will need to have the parts outside of your vault. If you have a PLM system that has to have an actual document, I would put the parts in the vault, but use them from the location outside the vault. You'll need to make sure people don't change the parts outside the vault.

This is gonna require some work.

Yeah, a lot of work.

Here's what I would recommend: Have someone go through and create all of the Toolbox parts you want to use as configurations. Then use the configured parts to autocreate Design Tables, and use the Design Tables to generate or populate part numbers and descriptions.

That's a lot of work up front, but if you really want to use Toolbox, Smart Fasteners and use them in the best way possible (with part nos and descriptions), I think that's the best way. The alternative is to enter in part nos and descriptions each time you make a new size, and then make sure everybody does it the same way every time.

And then comes the question of materials. If you use different material screws and you want that information to show up in the desc/part no, I would personally take the whole thing out of Toolbox and just make your own library. You could start with the configured and Design Tabled parts, but just put those in a library and forget about Smart Fasteners. If you make good use of patterned holes, Smart Fasteners really doesn't give you much anyway.

As you can tell, I'm a huge fan of Toolbox. It's nothing but a virus from a CAD administration point of view.

Well, you're gonna have to do one or the other (store separate parts or up-rev at each config addition). You might work around it by forcing the changed assembly to go back into the vault at the same rev, or you could use sub-revisions or versions... Well, actually, there is a way you could add a configuration to the assembly without even taking it out of the vault. You could use a linked design table. This would require you to keep the design table in some place outside of the vault, and when the assembly is taken out and opened, it reads the design table, and would add new configs/sizes. Of course you'd get -10 points for bad document management style, but it would do what you ask.

Anyway, good luck


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