I am working on an assembly I got from others, and they used toolbox parts. Is there a way to convert these parts into standard parts? Especially when I don't have toolbox?
I am working on an assembly I got from others, and they used toolbox parts. Is there a way to convert these parts into standard parts? Especially when I don't have toolbox?
Steve,
Have you tried the sldsetdocprop.exe
Found in C:\Program Files\SOLIDWORKS Corp xxxx\SOLIDWORKS\Toolbox\data utilities
You can use sldsetdocprop.exe to remove the toolbox state form components.
Did you try and open the part from the assembly or drawing and then doing a "Save As" in another directory???
John,
This works, but the part is still a toolbox part and we have had problems with toolbox parts giving us errors as we don't use toolbox.
Then save it as a parasolid ?
I can't find that program with that path. I'm using SW 2016
Exactly. Same problem. And as for a parasolid.... a big problem is that when I load the assembly, a 'size' is picked and I'm sure it's not what was originally designed. Parts are far oversized or undersized. I want to break the TB connection, and keep it broke.
Steven,
Try
Program files> solidworks corp>toolbox>data utilities.
Or just search for sldsetdocprop
What Jim wrote
Ok, found it. Used it. The parts still have the toolbox icon beside them. Even when I re-load the entire assembly.
I even tried this tool, and it says it can't find any toolbox part in the folder the assembly is in.
Steven Mills wrote:
Ok, found it. Used it. The parts still have the toolbox icon beside them. Even when I re-load the entire assembly.
I even tried this tool, and it says it can't find any toolbox part in the folder the assembly is in.
Ok. I believe you are using PDM?
If so, try with the TB part checked in and/or out. It's flakey. I've had it remove TB association with the part checked in and out at different times.
Not on the assembly I'm testing this on, I PnG it out of PDM.
If it helps, I've taken some parts still in the PDM and did a save-as into the folder I'm saving everything else in. some of those parts were toolbox parts.
Steven Mills wrote:
Not on the assembly I'm testing this on, I PnG it out of PDM.
If it helps, I've taken some parts still in the PDM and did a save-as into the folder I'm saving everything else in. some of those parts were toolbox parts.
Where are you seeing the toolbox icon besides the TB parts? In SolidWorks? SW may be referencing the vault items by default... Depending on your choices for file references, no?
They don't reference the toolbox parts after I do the save-as.
In the feature manager tree. It still displays as a toolbox screw 
, not as a part 
.
add a custom property: IsToolBoxPart for the value: 0
Then do a save as. Done
I hope this helps.
Dan
That worked. Had to close and re-load the assembly, but it worked. Thanks!
Steven Mills wrote:
They don't reference the toolbox parts after I do the save-as.
In the feature manager tree. It still displays as a toolbox screw
, not as a part
.
If the assembly is not in PDM, then we can try this:
Log-out of PDM and Exit entirely.
Does the assembly still reference the part as being a TB part?
No? good.
Yes? Close all of SW. Run the exe again. Make sure the property state is set to NO.
Chec the setting is NO
Does this fix it?
Yes? Good.
No? What do the file references say for the part location?
Thank you Dan. I have seen the istoolboxpart property referenced before but never was able to find it. Now I know why. I too have found a few former toolbox parts that have stubborn and will now know to use this.
Thank you
I already marked another as correct. But just so you know, I did do what you described, and the parts still came in the assembly as toolbox parts. I'm using SW 2016.
No problem. For an advanced method, I put it in my Property Tab Manager/Custom Properties for my parts: it works great:
Dan
It should still be there with 2016.
The default path would be C:\Program Files\SOLIDWORKS Corp 2016\SOLIDWORKS\Toolbox\data utilities
Found it. But it didn't work. The answer I marked correct did.
HOw do you do it? If i mark NO, is added some proprietary? Thanks!
Likely, when NO is selected, then the IsToolBoxPart property is set to 1.
When YES is selected, then the IsToolBoxPart property is set to 0.
Of course, we would need Dan (or someone else) to confirm.
It is a programming thing. In short the property has to have a 0 or 1, true or false. BUT anything with text is translated into a true, or 1 value. Does not matter if the text is 'Y' or 'N' or 'False' or 'True', all text values get changed to a value of 1.
add a custom property: IsToolBoxPart for the value: 0
Then do a save as. Done
I hope this helps.
Dan