Wacky Solidworks Toolbox Part Configurations
Brian Cannon
configurations and the actual configurations used in an assembly
either disappearing or changing in size when moved from one computer
or another.
I have observed the following which may be of use to some:
1) ToolBox part configurations are not saved in the model, but are
saved in the Toolbox database in the Toolbox Parts folder on the
computer (or network) where the part was created. So unless the
configuration happens to exist on the new computer you bring the part
to, the part will either not show up at all or revert to the default
size of the part on that computer.
2) There does not appear to be a way of easily transfering a
configuration of a toolbox part from ToolBox on one computer to
another, without overwriting any existing configurations in the
computer being transferred to. This is very unfortunate. It would be
nice if, for example, an assembly that had a Toolbox machine bolt of
say 4.25" long was moved to another computer that also had Toolbox
with the same bolt, but not that size in the database, would
automatically add the size to it.
3) In order to make Assemblies with Toolbox parts easily portable, one
has to either save all Toolbox inserted parts to the "Copiedparts"
directory (set in TooBox/Browser Configuration.../Document
Properties). This folder should be on a network, if there are multiple
users.
4) To make existing models portable with TB parts configurations, they
must all be saved individually as a new part in the Solidworks
Explorer under the Tools menu. This can be quite cumbersome.
Does anyone else have any ideas or quick solutions?
matt
No, but I have a couple corrections...
> 1) ToolBox part configurations are not saved in the model, but are
> saved in the Toolbox database in the Toolbox Parts folder on the
> computer (or network) where the part was created. So unless the
> configuration happens to exist on the new computer you bring the part
> to, the part will either not show up at all or revert to the default
> size of the part on that computer.
You're either confusing your terminology or you have a very basic
misunderstanding about how SW works. Toolbox configurations are definitely
stored inside the model, if by model you mean the Toolbox part. Only a
reference to the TB part config exists in the assembly (which is what I
guess you are calling the "model"). This is so the assembly knows which
part config to use.
TB parts install with only the default config, and more are created as you
specify new sizes.
What is stored in the database is the information to make each
configuration. TB parts are fully stand-alone parts, although configs may
be added to the parts.
Do you also think that an assembly built with Toolbox parts cannot be
opened by someone without Toolbox?
> 2) There does not appear to be a way of easily transfering a
> configuration of a toolbox part from ToolBox on one computer to
> another, without overwriting any existing configurations in the
> computer being transferred to. This is very unfortunate. It would be
> nice if, for example, an assembly that had a Toolbox machine bolt of
> say 4.25" long was moved to another computer that also had Toolbox
> with the same bolt, but not that size in the database, would
> automatically add the size to it.
You're right about not being able to copy configs between parts, but the
database doesn't have anything to do with it.
There are three ways around this:
- create all the sizes (configurations) available for all your TB parts.
- use the Copy Parts option
- copy the TB parts from one computer to the other, and make sure that the
assembly points to the right parts
> 3) In order to make Assemblies with Toolbox parts easily portable, one
> has to either save all Toolbox inserted parts to the "Copiedparts"
> directory (set in TooBox/Browser Configuration.../Document
> Properties). This folder should be on a network, if there are multiple
> users.
Let's say you want to put an assembly on a CD and mail it to a contractor
or archive it. All you have to do is go to File, Find References, and
Copy Parts, put them all in one blank folder, zip the folder and write the
CD. This has everything you need, including the TB parts, whether they
were created with configs or copied parts.
> 4) To make existing models portable with TB parts configurations, they
> must all be saved individually as a new part in the Solidworks
> Explorer under the Tools menu. This can be quite cumbersome.
I will grant this one IF all four of the following conditions exist (unless
the same Toolbox parts used in the transported assembly are already open
from the new computer's TB library.):
- The destination computer has Toolbox,
- the Toolbox parts on the new machine don't have the same configs your
Toolbox has,
- and the Tools, Options, File Locations, Referenced Files is set to read
from each and every Toolbox folder,
- Toolbox is installed in the same path on both machines
matt.
Brian Cannon
You have provided more useful information on how Toolbox works in one
posting than I have been able to find searching the net the past few
days. My points were my observations, being new to SolidWorks and
Toolbox.
Your are correct, I meant "assembly", not "part" as for the storage of
ToolBox information.
All your points are noted, and I am sure you have provide many others
with the information needed to help them decide the best way to use
ToolBox in there working environment :)
Brian
Rich
I work in a multi-user environment and we installed the toolbox
database on a network directory. We then make sure that no toolbox
parts exist on any local computers. In the SolidWorks\Toolbox folder
you can edit the toolbox.ini file to read from the network directory
that you established. This way everyone in the group is accessing the
same toolbox parts.
matt
If you're really interested in Toolbox data, I have a 70 page SW-written
white paper type document on my website which is very thorough. I doctored
it a little to add some info new in SW03. This covers topics like
customization, managing standards, Add My Parts Wiz, Smart Fasteners, and
multi-user installations.
There is one section that should be corrected. I don't know what possessed
me to insist on mapped drives on page 70. That's actually a really bad
idea. Must have written that late on a Friday night...
Anyway, read the disclaimer on pg 3, and if you find any (other) blatant
errors, please let me know.
If you're interested, it's on my website (http://www.frontiernet.net/
~mlombard), go to Rules of Thumb link, then Toolbox. There is a link to
the Toolbox Guide at the bottom of that page.
matt
b_ca...@westmillindustries.com (Brian Cannon) wrote in
news:67791a20.03040...@posting.google.com:
--
matt
http://www.frontiernet.net/~mlombard
remove the "_" from email address
matt
news:86d91d49.03040...@posting.google.com:
Did you also make the "read-only" settings? If you don't, what happens is
that the first one to open an assembly with a TB part in it gets write
access, then if someone else needs to make a new config of that part, he's
"screwed" so to speak.
The settings are found on the Toolbox menu, Configure Browser, Browser tab,
Document Properties page. Turn ON "Insert documents as read only" and
"Always change read only status of document before writing". This makes
sure that all toolbox parts are loaded read only, then if you need to make
a config it is changed to write access, saved, then changed back.
Brian Cannon
> If you're interested, it's on my website (http://www.frontiernet.net/
> ~mlombard), go to Rules of Thumb link, then Toolbox. There is a link to
> the Toolbox Guide at the bottom of that page.
I have visited your site as above and find it extremely useful! Tons
of information, just what I have been looking for!
Brian
Rich
Yes. Our VAR actually clued us in on these settings. I forgot to
mention them previously.
Einar Knudsen
After my colleague opened my network-stored assembly on a fresh install of SolidWorks 2020 SP5.0, some parts have mysteriously changed size. These are ISO parts that were taken from the toolbox.
When I right-click on the components, the "Edit Toolbox Components" option is missing.
The solution presented in this link did unfortunately not work for me. me https://forum.solidworks.com/thread/60483
I can't seem to change the size of these ISO components, unless I treat them as custom parts. I'd like to avoid this as I'm not quite ready to redesign all the gears and screws simply imported from the ISO library.
Einar