Changing a part template 1

[VELCROW]

I have a part that used an incorrect template so plane names, custom properties, etc. are not right.

Can I switch the template after the part is made?

This thread thread559-230898 refers me to a macro that lets me switch Drawing templates, but not Part templates.

If I can't switch the template, is there a way to grab all the features from the part and move them to a new part that uses the correct template?

Thanks,

Steve

 

[CorBlimeyLimey]

The Copy Custom Info or mac_copydoc listed in faq559-1429 should help.

I'm not sure about the Ref plane names though.

 

[VELCROW]

Thanks CB, that covers custom properties, which is the most obvious change. But there could be many other differences (e.g. Ref plane names) that will get me in trouble down the road. Off the top of my head, anything in the Document Properties tab of Tools>Options could be different.

If I could replace the template, or copy all the features to a new part, I wouldn't have to worry.

Thanks,

Steve

 

[CorBlimeyLimey]

If you have customised the options under a specific standard, that cusomisation can be saved to an external file for application to other documents.

 

[fcsuper]

The simply answer is no if you want every detail, but the links from CBL will cover most stuff.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[Gupta65]

Look here, I believe this is what you need:

http://gupta9665.wordpress.com/2009/08/21/how-to-change-sw-file-system-options/

Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0

 

[VELCROW]

Deepak,

Thanks for posting. Unfortunately, according to the notes in the Excel file, "It works only with drawings".

Now, it also says it "may be enchanced easily to work with other document types and even with the Solidworks system options", but my VBA is not that good, and the code is commented in German.

Isn't there some way to copy features from one part to another?

 

[CorBlimeyLimey]

Ignore the "It works only with drawings" comment. It does work with parts and assys. Use the worksheet tabs to switch types.

 

[fcsuper]

VELCROW,

No, there's no way to do what you want in the way that you want. There are other options. If you wish to copy features, you can save them from your source file to your design library, and then insert them into your other part. There's no way to automatically rename stuff or do a lot of what you are asking without some VERY specific API. You'll spend more time writing the code then just manual making the changes in your new file.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[VELCROW]

Thanks to all for your help. This will get me 99% there, which is a lot better off than I was before.

 

[HercalloY]

velcrow,

This may give you what you want... i've done it a couple of times to achieve a similar thing you seem to want to do...

Create a new part using your desired part template...

Go to pulldown menu "Insert"
Then "Part..."
Select the part you wish to update...
In the "Insert Part" property manager select "Break link to original part" check box.
Select the origin to insert it at that point.

Now you should find SW has inserted the part and zoomed extents also having created a folder containing all the features of that part you inserted. to make it "normal" you can simply delete the folder and all features will be at the root level. At this point you can save it off as the same part number and overwrite existing (tho i'd recommend checking the part out thoroughly in case, before doing that).

I havent found any problem with this yet so it seems to do what i want to which seems to be exactly what you want to do.

 

[VELCROW]

That seems to do it. It doesn't copy the custom properties, but the earlier posts cover that.

 

[fcsuper]

"Break link to original part"

It never truly breaks the link though. The file will always remember where it came from. This can be an issue when using PDM.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[VELCROW]

We're small enough that we don't use PDM, so it is not an issue. Even if we do go to PDM eventually, we can use this until then.

 

[Gupta65]

Velcrow,

The macro listed in this link (

http://gupta9665.wordpress.com/2009/08/21/how-to-change-sw-file-system-options/)

works for part, assembly and drawing.

Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0