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
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
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
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
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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