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$PRPWLD:"Description" not working in a note in a weldment part.

Question asked by Robert Stewart on Feb 24, 2018
Latest reply on May 23, 2018 by Alexandre Gragnano

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In 2017 and earlier, we used a note and this macro: https://www.javelin-tech.com/blog/2013/05/link-solidworks-custom-property-to-note/#.WH0gz1UrKCg

to transfer the following properties to our BOM:

For weldment parts: $PRPWLD:"Description"x $PRPWLD:"LENGTH" LG.

For sheet metal parts: $PRPWLD:"Sheet Metal Thickness" X $PRPWLD:"Bounding Box Width" X $PRPWLD:"Bounding Box Length" LG.

Some of the properties aren't transfering to my notes in 2018, the note is just blank (the property is still in the note, but the value is passed). I can't figure out the problem. It's driving me crazy. I think it has to do with the new Linked Properties, but they aren't in the What's New Document so I can't figure them out either!

$PRPWLD:"Description" Works at first, then disapears after properties/parts are edited

$PRPWLD:"LENGTH" Seems to work all the time

$PRPWLD:"Sheet Metal Thickness" I haven't test yet Sheet Metal Properties still appear to be working

$PRPWLD:"Bounding Box Width" I haven't test yet Sheet Metal Properties still appear to be working

$PRPWLD:"Bounding Box Length" I haven't test yet Sheet Metal Properties still appear to be working

I need to start a case with my VAR, but yet again, SW has broken yet another workaround without fixing the root problem.

There were multiple threads in this years top 10 list voting that Deepak Gupta started for this issue. I can't find them now though. Deepak, any ideas?

Edit: Added a screen shot of my Weldment Custlist Property window.

Hit End twice when you open the template, because the macro feature won't load without the macro file.

You need to right click on Annotations > Display Annotations to show the note. It's hidden in the template.

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Weldment Cut List Screen Shot.JPG90.2 KB
Structural Member - 2018.PRTDOT.zip60.4 KB
Structural Member - 2017.PRTDOT.zip58.3 KB

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Alexandre Gragnano May 22, 2018 11:54 AM

Hi Rob,

I am currently experiencing a similar problem:

- Open SolidWorks 2018 (any SP)

- Create new Part document

- Create new sketch on face plane

- Create a line in this sketch

- Create a sweep function with circular profile to obtain a bar

- Add "Weldment" function to feature manager

- Edit the generated cutlist custom properties

- Add a custom property named "CUSTOM" with value "CUTLIST" and validate

- Edit the part document custom properties

- Add a custom property named "CUSTOM" with value "PART" and validate

- Save the part document

- Create a new drawing document

- Add a face view of the part into the sheet and validate

- Add an empty note attached to the bar and validate

- Right click on the empty note > Edit text in window

- Write : $PRPWLD:"CUSTOM"

Expected result : CUTLIST

Obtained result : PART

- Return to the part document

- Edit the part document custom properties

- Modify the name of the "CUSTOM" property to "CUSTOM2"

- Come back to the drawing document

Expected result : CUTLIST

Obtained result : CUTLIST

Conclusion: the weldment cutlist properties are overridden by the part document properties of the same name.

In your case, the cutlist properties which are not "transfered" to your notes are properties which exists (natively or not) in your part document properties.

Regards,

Alexandre

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Robert Stewart @ Alexandre Gragnano on May 22, 2018 12:06 PM

My VAR created a SPR for my problem above. It is SPR #1059739. Please vote for it and let me know what number they assign to your issue and I'll vote for it as well.

Thanks for the response.

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Tom Gagnon May 22, 2018 12:27 PM

Rob -

We've been experiencing a very similar issue as well. I've just been working around it when encountered, as it is not consistent in all cases.

I have weldment component parts, which have Custom Property named Description. I have the nearly identical weldment callout saved as a Library Note: "$PRPWLD:"Description", $PRPWLD:"LENGTH" LG." When making a drawing of the part, we attach these note leaders as needed to views, and can then stack same ones so it appears as one note, for example, with three leaders pointing at three identical bodies.

For only the past two weeks, about 40% of my parts do not correctly show the $PRPWLD:"Description" of the body, but instead it returns the part's Description custom property. When it does this, it mis-performs consistently to all bodies within that same part and linked leaders added to the drawing.

To workaround and push through, all I do is rename the part's Description custom property to NotDescription instead. Then when I return to view the drawing, the weldment properties carry through correctly. However, once the part's description is called for in a different context, I'll likely go back and either re-rename it back or just re-add the Description custom property. It is a brief repair that works for us because the unique custom fab detail is completed and published to PDF, so it matters less to me if the SLDDRW file does not update correctly after it is rendered.

What didn't work: I tried updating cutlist in the part. That did not fix anything.

While I agree this isn't how it should behave, it is a very minor hiccup compared to some other issues we experience. I am not chasing it down for VAR support or xR#. I'd be happy to add my vote to your similar issue, without duplicating one of my own.

Installation ref: 2018 SP2, Win 7 Pro

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Robert Stewart @ Tom Gagnon on May 22, 2018 12:31 PM

Thanks for voting. This is a big deal to us because we have 1000+ library features and templates set up and working in 2017 and prior. This and one other Custom Property "regression" have stopped us from updating to 2018.

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Alexandre Gragnano May 23, 2018 3:07 AM

According to my tests, if you start to work from part documents originally created from SW 2017, you can retrieve your custom properties.

The problem probably lies into the file initialization, I think into the data structure of custom properties because after saves onto SW 2018, the custom properties are always accessible.

A temporary solution consist to create every new part document from SW 2017.

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5 Replies

Alexandre Gragnano May 22, 2018 11:54 AM
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Correct Answer
Hi Rob,

I am currently experiencing a similar problem:

- Open SolidWorks 2018 (any SP)
- Create new Part document
- Create new sketch on face plane
- Create a line in this sketch
- Create a sweep function with circular profile to obtain a bar
- Add "Weldment" function to feature manager
- Edit the generated cutlist custom properties
- Add a custom property named "CUSTOM" with value "CUTLIST" and validate
- Edit the part document custom properties
- Add a custom property named "CUSTOM" with value "PART" and validate
- Save the part document
- Create a new drawing document
- Add a face view of the part into the sheet and validate
- Add an empty note attached to the bar and validate
- Right click on the empty note > Edit text in window
- Write : $PRPWLD:"CUSTOM"

Expected result : CUTLIST
Obtained result : PART

- Return to the part document
- Edit the part document custom properties
- Modify the name of the "CUSTOM" property to "CUSTOM2"
- Come back to the drawing document

Expected result : CUTLIST
Obtained result : CUTLIST

Conclusion: the weldment cutlist properties are overridden by the part document properties of the same name.

In your case, the cutlist properties which are not "transfered" to your notes are properties which exists (natively or not) in your part document properties.

Regards,
Alexandre
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- Robert Stewart @ Alexandre Gragnano on May 22, 2018 12:06 PM
  Mark Correct
  Correct Answer
  My VAR created a SPR for my problem above. It is SPR #1059739. Please vote for it and let me know what number they assign to your issue and I'll vote for it as well.
  
  Thanks for the response.
  Like • Show 3 Likes3
  Actions
Tom Gagnon May 22, 2018 12:27 PM
Mark Correct
Correct Answer
Rob -
We've been experiencing a very similar issue as well. I've just been working around it when encountered, as it is not consistent in all cases.

I have weldment component parts, which have Custom Property named Description. I have the nearly identical weldment callout saved as a Library Note: "$PRPWLD:"Description", $PRPWLD:"LENGTH" LG." When making a drawing of the part, we attach these note leaders as needed to views, and can then stack same ones so it appears as one note, for example, with three leaders pointing at three identical bodies.

For only the past two weeks, about 40% of my parts do not correctly show the $PRPWLD:"Description" of the body, but instead it returns the part's Description custom property. When it does this, it mis-performs consistently to all bodies within that same part and linked leaders added to the drawing.

To workaround and push through, all I do is rename the part's Description custom property to NotDescription instead. Then when I return to view the drawing, the weldment properties carry through correctly. However, once the part's description is called for in a different context, I'll likely go back and either re-rename it back or just re-add the Description custom property. It is a brief repair that works for us because the unique custom fab detail is completed and published to PDF, so it matters less to me if the SLDDRW file does not update correctly after it is rendered.

What didn't work: I tried updating cutlist in the part. That did not fix anything.

While I agree this isn't how it should behave, it is a very minor hiccup compared to some other issues we experience. I am not chasing it down for VAR support or xR#. I'd be happy to add my vote to your similar issue, without duplicating one of my own.
Installation ref: 2018 SP2, Win 7 Pro
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- Robert Stewart @ Tom Gagnon on May 22, 2018 12:31 PM
  Mark Correct
  Correct Answer
  Thanks for voting. This is a big deal to us because we have 1000+ library features and templates set up and working in 2017 and prior. This and one other Custom Property "regression" have stopped us from updating to 2018.
  Like • Show 2 Likes2
  Actions
Alexandre Gragnano May 23, 2018 3:07 AM
Mark Correct
Correct Answer
According to my tests, if you start to work from part documents originally created from SW 2017, you can retrieve your custom properties.
The problem probably lies into the file initialization, I think into the data structure of custom properties because after saves onto SW 2018, the custom properties are always accessible.

A temporary solution consist to create every new part document from SW 2017.
Like • Show 2 Likes2
Actions

$PRPWLD:"Description" not working in a note in a weldment part.

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