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Standard part keeps referencing old part 1

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cinnamongirl

cinnamongirl

Mechanical
Jan 18, 2011
106
I was given an assembly with a standard part bearing. I modified and saved this bearing under a different name in the assembly's home directory. I inserted the part in the assembly, however every time I open it the assembly keeps referencing the original part. I work around this by opening the modified part first and the assembly next. How can I update the assembly so that it references the new part?

Also, how do I create a part from scratch to show as a standard part in the model tree?
 
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Original part= needle roller bearing_niu_ai
Modified part= SJ 7174 SS

I looked and noticed that the original part name also appeared on the configuration tree (in parenthesis right after "Default"). I thought that might have been the cause of the problem so I deleted it, but it's still loading the original part.
 
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Yes, I do and I still keep getting the old part when I close and open the assembly (unless of course I have the new part open).
 
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Close all assemblies and parts
Go to File > Open
Select (but don't open) the assy
Select the References option
Double click the referenced part in the References box
Browse to and select the required part > click Open
Click OK
Open the assy and Save
Close the assy
Open the assy and check the part is correctly referenced
 
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No, selecting the References option is not working, but thanks anyway.

I recently noticed that when I open the assembly it appears to be correct for one second, but then it asks me to rebuild and that's when it switches to the old part. I'm guessing this has something to do with being a modified standard part.
 
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By "standard part" do you mean a part from the toolbox? Try >>Tools >>options >>system options >>Hole Wizard/Toolbox, and uncheck "Make this folder the default search location for toolbox components."

Joe
SW Premium 2011 SP0.0
Dell T3500 Xeon W3505 2.4Ghz
6.0GB Win7 Pro x64
ATI FirePro V5800
 
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Yes, thank you! It worked! I had renamed the part and saved it in the assembly's directory and it still kept grabbing the original part from the toolbox. I even tried placing the renamed part in the toolbox folder but the assembly kept selecting the old part. But everything seems fine now.

But just in case, how do I convert this toolbox part into a regular part? (it's showing up with a bolt symbol in the model tree) Other people have access to the assembly so I would like to take some preventive measures. Thanks again.
 
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How about trying to do a replace part in the assembly? Right click on the old part in the feature tree. Browse to the new part and replace all instances. Then save the assembly and close down SW.

BTW, are you using a PDM system? You didn't say what release or hardware you are running.

TOP
CSWP, BSSE
Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."
 
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I did replace the part in the assembly, but each time I opened the assembly it referred back to the original part. That's why I had to have the renamed part open first so that the assembly would grab it. I would like to make this part show up as a regular icon on the assembly model tree (it's a bolt right now).

And no, no PDM here, just sharing the files from a networked workstation. And we are running SolidWorks 2011 x64 Edition.
 
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I think that you can use C:\Program Files\SolidWorks Corp\SolidWorks\Toolbox\data utilities\sldsetdocprop.exe to remove the flag that tells SW that a part is a toolbox part.

I have some recent experience which leads me to believe that when a toolbox part is contained in an assembly, that SW stores additional information about that part in the assembly which allows it to recreate the part from the toolbox. I would recommend clearing the toolbox flag, opening and resaving the assembly. Hopefully that will make the assembly forget that the part was once a toolbox part.

The setting that JMarv suggested appears to affect weather or not SW looks for the part in places other than the toolbox before it generates the new one from the toolbox.

Eric
 
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I agree with Eric's explanation and suggestion to run sldsetdocprop.exe on the offending part. It's my understanding that you need to make sure that you have no files open when you run that utility.

Here are a couple discussions on the subject:

Joe
SW Premium 2011 SP0.0
Dell T3500 Xeon W3505 2.4Ghz
6.0GB Win7 Pro x64
ATI FirePro V5800
 
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Hi, cinnamongirl:

Replacing a part is very simple. Try to follow SW help menu on replacing a component part.

Alternatively, you can kill the old one in your assembly, and re-insert the new one.

Good luck!

Alex
 
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sldsetdocprop.exe worked! It took a few attempts but eventually I was able to make the toolbox icon go away. Now the renamed part loads automatically every time.
 
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