Update parametric notes 1

[markbreneman]

I have a set of drawings with parametric text blocks linking to the parts volume, weight, ect. and I am now haing to go back through and rename all the parts, unfortunately when i use solidworks explorer to rename it does not update the changed parameter drawing; so althought the part and the assembly relations are maintained fine, the parametric relations in the drawing can't find the part be cause of the rename. Any help?

 

[ctopher]

When you did the rename, did you have the box checked "Update where used"?

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[markbreneman]

Yes I had the update where used checked. It just kind of sucks. I have a feeling that the search where used function goes deep enough to find drawing and views which use the model but not notes or noteblocks ect.

 

[ctopher]

Try open the drawing, then do "Ctrl-Q"?

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[markbreneman]

Are you sure you mean Ctrl Q. Ctrl Q quits the program. if you are trying a reload, I've tried that.

 

[ctopher]

Ctrl-Q is a force rebuild...unless you changed its settings.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[CorBlimeyLimey]

Ctrl Q is the default setting for a forced rebuild. If your Ctrl Q is quiting the program then someone has changed the keyboard shortcut.

 

[markbreneman]

Tried the force rebuild as well, no luck. Any other suggestions. I mean all the parameter text stays in the block it just shows up as text with the previous part name.

 

[ctopher]

Try:
Open drawing, browse to drawing file and click on the drawing, select the "references" button at lower-right. Change the location to the new renamed file.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)

 

[handleman]

Did you create these "parametric notes" by typing in the part name? If so, you will not be able to get them to update automatically. Only notes linked to the "model specified in sheet properties" or to the "model in view to which annotation is attached" will update automatically.

-handleman, CSWP (The new, easy test)

 

[DesignerGuy16]

Are these notes excel sheets perchance? Or actual links?

If they're links it should be linked to a property/variable, and that should be specific to the model, and have nothing to do with the file name.

IE. I use Description as a custom property, so to show in title block I make a link using $PRPSHEET:"Description".

If I drop a drawing view onto that sheet, the first part will fill out that description. If I drop a different part it won't update unless the first view goes away.

Now if you setup that note to a block with the same parameters and insert the block with the 2nd view selected it will link to that particular view. (I think this is more up the alley of what you're doing)

Now changing parts shouldn't change the link as long as you use SW Explorer to change the names using where used and it updates the SLDDWG AND the SLDPRT/ASM. That's because the block isn't linked to a filename, it's linked to the view, and changing the filename won't change any variables/properties so it will still push through.

James Spisich
Design Engineer, CSWP

 

[handleman]

Please check out thread559-221489. I am guessing your issue is the same.

-handleman, CSWP (The new, easy test)

 

[markbreneman]

Handleman pointed me in the right direction, I had a custom property, when i could have just a PRPsheet property. Thanks everyone

 

[ctopher]

I guess it was a simple fix. I thought is was something else going on. Screen shots or more detail would help more next time. Good to know handleman's link worked for you.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)