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SW bug: Link between parameters: Part’s GV->Custom Property->Sketched Text isn’t working!!!

Question asked by Vladimir Urazhdin on Apr 26, 2019
Latest reply on Jul 16, 2020 by Elmar Klammer

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On the sample below shown a Part with Custom Property “Description” linked to a couple Global Variables: “H”, “L”, “D”.

Equation manager looks good:

Part’s Custom Properties:

Now I want to laser engrave on the part’s face the Custom Property “Description”.

This is the link between Sketched Text and Custom Property:

A discouraging result:

It looks like on the Sketched Text instead of Evaluated Value SolidWorks displays the Text Expression (the source code)….

So far I’m not able to figure out the spin around to resolve this issue.

The Part to play with is attached.

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sw bug.SLDPRT.zip900.4 KB

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Jackson Wiebe Jul 10, 2019 12:33 PM
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Also have this issue.
The property isnt evaluating properly.
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Glenn Schroeder Jul 10, 2019 12:43 PM
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I bypassed the global variable step and linked a new property directly to the dimensions, then linked the sketch text to this property, and it worked fine.
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- Vladimir Urazhdin @ Glenn Schroeder on Jul 10, 2019 4:02 PM
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  GV may have nothing to do with any dimensions. Examples: Part-, Project-, ECN numbers and so on. In some cases, to spin around, I had to create a virtual sketch with virtual dimension and link GV -> virtual dimension -> property.
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Kevin Chandler Jul 10, 2019 12:53 PM
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Hello,

Although I don't have workaround or a remedy, it appears the linked text is being pulled from the "Value/Test Expression" column and not from the "Evaluated Value" column.

None of the other properties display correctly either, but if you just type text in the "Value/Test Expression" column, it displays. So this is the issue I believe you're facing.

This behavior doesn't seem correct.

Perhaps your VAR can escalate this issue to SW for you and perhaps tell you if there is an existing SPR for this.

Kevin
(SW2018 sp2)
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- Vladimir Urazhdin @ Kevin Chandler on Jul 10, 2019 4:20 PM
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  I already did it.
  Below is the copy of my VAR response:
  
  "Hi Vladimir & Mike,
  Yes, you are running into an issue that is in SolidWorks SPR pool. We associated you to the SPR over a year ago. It has not been corrected.
  The attached is a file that shows a work around. I drive the property with actual dimensions.
  This is how we worked before global variables.
  BTW, I worked the problem in both SolidWorks 2018 and 2019. No difference.
  Sorry I don’t have better news.
  Best Regards,
  Tom Landrey
  Partner - GM"
  
  This is the ERROR! And nobody from SW development team takes care about it!!!
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  - Peter Brinkhuis @ Vladimir Urazhdin on Jul 14, 2020 3:31 PM
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    I'm still having this issue in SW2020SP2...
    
    Edit: After hours of digging I found another workaround. It works when you add the text in a note within the sketch, instead of a sketch text In a block also works.
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    - Elmar Klammer @ Peter Brinkhuis on Jul 14, 2020 1:40 PM
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      Hi Peter,
      
      That has been really unpredictable from my experience. Rotating the view and you got nothing but issues. Notes being linked to annotation views. It would be really nice to be able to link text into sketches without using sketch text. Is this working in 2020 now. 2017 was a smash…
      
      Elmar
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      - Peter Brinkhuis @ Elmar Klammer on Jul 14, 2020 3:33 PM
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        Hi Elmar,
        
        I don't understand what you're looking for exactly.
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        Elmar Klammer @ Peter Brinkhuis on Jul 15, 2020 1:18 AM
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        I had a situation where I wanted to add text notes (not sketched text) in a sketch just like you mentioned. I needed to show information in various drawings view. A simple sketch. Some rectangular boxes with description. The sketch font scaled to suit my sketch size. First I couldn't use leader text. SW would tell object with some sort of error message "due to blah blah blah..text size can't be blah blah". Then I couldn't position notes to stay. Anyways I just aborted the idea and worked with drawing blocks instead. But since you mentioned that you used regular text instead of "sketch text" I thought I'd ask how you did that. I know it sounds rather simple. But in 2017 I was not able to place text annotations inside a sketch that would stay put where I placed them. I can't specify text size that maintains it's size. I was curious to know whether you knew how to place regular text inside a sketch that behaves just like sketched text.
        
        Elmar
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        Peter Brinkhuis @ Elmar Klammer on Jul 16, 2020 9:00 AM
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        I thought I added notes to a sketch, but as it turned out, I added them to the part. I ended up creating a block that contains a single note, that contains multiple custom property values. This works.
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        Elmar Klammer @ Peter Brinkhuis on Jul 16, 2020 11:51 AM
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        Hi Peter,
        
        Thanks for the info. I have used the block trick before but honestly I was hoping you had the magic trick where I can use simple text notes in part sketches. Too bad. Well maybe one day. Not sure why it is so hard to add text inside a sketch.
        
        Thanks anyways.
        
        Elmar
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  - Josh Brady @ Vladimir Urazhdin on Jul 14, 2020 11:35 AM
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    Vladimir Urazhdin wrote:
    
    I already did it.
    Below is the copy of my VAR response:
    
    "Hi Vladimir & Mike,
    Yes, you are running into an issue that is in SolidWorks SPR pool. We associated you to the SPR over a year ago. It has not been corrected.
    The attached is a file that shows a work around. I drive the property with actual dimensions.
    This is how we worked before global variables.
    BTW, I worked the problem in both SolidWorks 2018 and 2019. No difference.
    Sorry I don’t have better news.
    Best Regards,
    Tom Landrey
    Partner - GM"
    
    This is the ERROR! And nobody from SW development team takes care about it!!!
    Yup... Every bug has to be prioritized. If the number of users impacted is low, and there is a straightforward and relatively obvious workaround, yes. Nobody cares about it. It's also possible that even though it looks like a simple thing, it would take significant rewrites or changes to other parts of the program.
    
    It's not like they're sitting around going "ain't no bugs on me" and twiddling their thumbs, but they can't squash them all. They have to allocate resources where they have the most impact.
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Damir Galic Jul 15, 2020 1:23 AM
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This is also a problem in drawings. If you link titleblock or BOM to property values sometimes it doesn't get evaluated.

Why they don't fix it? I guess because it would slow down solidworks pretty much.
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