How do I convert a toolbox item to a non- toolbox item? I want to save a toolobx item as a standard part file to modify and check into the vault.
Run "SLDSETDOCPROP.EXE" which is in your solidworks\toolbox\data utilities directory. Set the part to NO
I'm having an interesting problem, even after I used that feature.
Even after I set the "IsToolboxPart" variable (or whatever its called) to "no", the parts still occassionally load as toolbox components when they are part of an assembly file that I open.
(Or at least: you still see the Toolbox icon in the feature manager and you can't configure the part)
The funny thing? I can suppress the parts, then unsupress them, and everything is gravy.
But then, even after I save the assembly (and the fastener) after the correction, the next time I open the assembly, it's the same old thing all over again.
Ain't that a b....
Curious, what was it doing before you ran this command?
John, what version and service pack of Solidworks are you running?
In general, it seems to happen like this:
Truth be told, it usually happens long enough after the assembly was first created, and frequently enough with a range of assemblies, that I'm not certain at all how step #4 comes about. At first, I thought it just happened with upgrades/service packs, but it just kept happening with other assemblies. At this point, I'm at a loss.
Edit: I'm sure it's probably something relating to search paths and toolbox locations. If I get a chance to investigate that today, I'll update with a more clear picture of what my system is doing right now. In fact, I'll just assume that that's really the initial problem: we're still early in our SolidWorks implementation and we don't have our PDM system set up yet.
You might want to look into running the Rx tool
and sending that file to your VAR for them to forward on to Solidworks.
I saw in another forum that the user needed to move the files out of his "toolbox" location. Just a thought.
Has anyone found any solution for that?
The application and method suggest above should work for you. In case it is not working, move the required toolbox parts to a different location and then run the application and check.
In addition to that make sure the part file and assembly containing these file must be close during running the "SLDSETDOCPROp.exe" utility.
This "feature" has been driving me nuts too! I've been deleting all my toolbox fasteners and remodelling them because they keep randomly resetting themselves.... even in SW2011 SP4.
Even with the SLDSETDOCPROP function, it's not exactly clear what you are supposed to do.
"Property State: Yes" and "Property State: No" are not exactly meaningful are they? I assume they intended mean "Set as toolbox item: Yes" etc...
C'mon Sldwx, surely there is an easier way to do this, or just delete the entire toolbox functionality because its more trouble than it's worth.
Matt Swan wrote: I assume they intended mean "Set as toolbox item: Yes" etc...
Matt Swan wrote:
I assume they intended mean "Set as toolbox item: Yes" etc...
You assumed it right.
It may sometimes happen when you're working in networking or have same/similar files in different location/folder that might had been open while your assembly is open which sometimes doesn't set the property correct or SW uses the other available file in memory. So make sure you're not running SolidWorks while using the SLDSETDOCPROP function.
David Mandl wrote: In general, it seems to happen like this: Create new part from toolbox part (via "save as copy")Insert new part into assemblyIndeterminate amount of time wherein the assembly refers to the new partOne day, the assembly opens and you've got the generic version of the original toolbox component sitting there. Truth be told, it usually happens long enough after the assembly was first created, and frequently enough with a range of assemblies, that I'm not certain at all how step #4 comes about. At first, I thought it just happened with upgrades/service packs, but it just kept happening with other assemblies. At this point, I'm at a loss. Edit: I'm sure it's probably something relating to search paths and toolbox locations. If I get a chance to investigate that today, I'll update with a more clear picture of what my system is doing right now. In fact, I'll just assume that that's really the initial problem: we're still early in our SolidWorks implementation and we don't have our PDM system set up yet.
David Mandl wrote:
Today's activity in this thread reminded me: After all this time, I never updated with my findings from some of the tests I ran regarding this subject.
I can say with absolute certainty that your search paths and toolbox locations are a major contributing factor to this problem. Any time someone opens an assembly with a different toolbox filepath setting than the rest of your network, you're asking for trouble. (This is, of course, why we should all be using copy options to create our standard network settings and why we give dirty looks to anyone in our departments who tries to mess with them)
As for the files where the problem would return even after I set the properties correctly: all I had to do was delete them from the assembly, save, then come back later and re-insert the fasteners. It's a little more work, but it did give me clean assemblies.
This is a known bug in some versions of SW.. was really frustrating. This may help:
Read the link and sounds like its an on going issue.
Not sure how to convert all of our current files from Toolbox document to Solidwork part files?
I know there were issues at that point in time. I threw it at you in case the procedure might
work now being a couple of version ahead now. I personally just like using toolbox as a benchmark
for creating my own hardware library. Have you tried doing save as copies of the toolbox parts?
I had the same issue trying to check in a special washer that was actually made from a part created by the toolbox. I couldn't break the link to the toolbox.
Finally I created a mirrored part, breaking the link to the original part and then deleting the mirrired feature. I ended up with an independent part that could be checked in to the vault.
According to SW, there is a bug that once an assembly has toolbox parts in it, it there is no way sure-fired way to remove them short of making a new assembly. You can run SLDSETDOCPROP on the parts. One a part is changed, you have all the pars in the same folder as the assembly and you DO NOT have matching parts in the path of where SW thinks your toolbox part are, you can open the file and work like normal. The icon may (or may not) still be wrong but according to SW there is no other harm. To be sure you have it correct, set all parts to "resolved", go to File | Find References and make sure all files are local to the assembly folder.
If you open each part first and then open the assembly, the icons will be correct but this will not stick. If you open just the assembly later, the icons will be back to toolbox. I say this lightly as this is not "always" true. Sometimes it will fix itself. I have only seen this on small assemblies and have not figured out what I did to make it correct.
FYI - Files have one of three states:
I have seen cases where a part set as swDmToolboxCopiedPart required one to change it to "Yes" twice before it was really changed. I ended up writing my own program (with a MUCH better UI) that calls the same function the swdocumentmgr library.
Toolbox parts also have another hidden property called "IsFastener" but so far, I have been able to change this value. There is an undocumented feature called "Allow to spin" that I believe this feature is tied to but I have not confirmed this.
Hope this helps.
FYI - I have an improved tool to clean up toolbox parts. It will clean up an entire hard drive if you like. Does samething but with a better UI
<updated with rev 1.4>
Take a tool box item (ex: bolt) in to an assembly file and open the part separately as a part file.
Click save. Save file dialog box will appear. There you have a check box at the bottom left corner.(see figure below) Click on it and hit save button.
Open the saved file and do whatever the changes you need.
Thanks a lot. You helped me a lot.
I had few parts with some toolbox status. And I couldn't use anymore (since when?) the "Right-Mouse-Click" configure component on those parts in an assembly. Now that my parts are fixed, I don't meet that issue anymore.
Very nice application. And on an SSD, it goes so quick... You should be a very good developper.
Make sure that in your System Options > Hole Wizard Toolbox > "Make this folder the default search location..." is unchecked.
This fixed my issue. I know I've unchecked that box before & somehow it gets re-checked. I think SolidWorks has a ghost in the machine. I have lots of other issues similar to this, where I have settings set a certain way & then one day I start up SolidWorks and one of the settings will mysteriously have reset itself. I also have custom toolbars reset themselves from time to time.
It is really annoying.
This fixed my issue too.
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