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In a new sheet format, how can I set an automatic field that displays the mass of my solid part?

Question asked by David Bracke on Apr 14, 2020
Latest reply on Jul 3, 2020 by David Bracke

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In Solidworks 2017, I have figured out how to manually do this:

After modeling the solid part, make the drawing,

1) add a Note,

2) select Link Property to enter Link Property menu,

3) click File Properties to enter the File Properties menu,

4) set a Property Name [ANY_NAME],

5) select Type "Text",

6) enter Value / Text Expression of "SW-Mass@[SOLID_PART'S_FILE_NAME_GOES_HERE].sldprt",

7) click OK to go back to Link Property menu,

8) select Property Name [ANY_NAME],

9) click OK.

It's not exactly quick. Now I'll have to do this ... several hundred times, and I'm trying to figure out what syntax I need to make it happen automatically. I think that step 6 is where there could be a solution.

Specifically, I have made a custom sheet format with my name signed and a few other details set in advance, so I can go directly from my solid model to a halfway-finished sheet. I want the mass value to pull automatically from the solid model. I know there are some other syntax lines that do the same, such as $PRPSHEET:{Material} and $PRPSHEET:{Finish}, so I think there must be a similar way to call the mass value.

I have tried $PRPSHEET:{Mass} and have had no luck. Does anyone know another possibility?

Or maybe I'm approaching this from the wrong point-of-view and there is an easier answer?

Thanks

-David

EDIT: Okay, I am blind. This feature is already built into the default templates, labeled as "weight", and it is blank unless you set a material for the 3-D model. I suppose my question should be rephrased - can I call any other information from my solid model in the same way?

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Glenn Schroeder Apr 14, 2020 3:56 PM
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I'm afraid I didn't follow all of your steps, or where you're doing them. You can create custom properties in a model, and then reference these properties in a Drawing. I've been using SW for 35 - 40 hours per week since 2009 and I haven't bothered to learn the syntax for any properties.

There's a wide selection of model characteristics that can be linked to a property within the model with the drop-down...

...and in Drawings I use the "Link to Property" icon in the drawing note's property manager.

See What's the difference between a sheet format and drawing template?, starting where shown below.

I have Styles saved for my most often used Notes, so I either use those, or copy and paste, so I don't need to repeat the process every time I want to link to the same property in another Part. I hope this helps, and be sure to ask if you have other questions or need clarification.
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- David Bracke @ Glenn Schroeder on May 4, 2020 8:54 PM
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  Hello, Glenn,
  
  I'm sorry it took me a while to get back to you. I've been working on a few (dozen) other projects at work ...
  
  So I see the very first image you have posted in your reply. You have pulled up the File Properties menu, under the Custom tab, and you have a drop-down menu in the third column. I can't get that drop-down menu to show any options at all (there is one option, and it is blank ...)
  
  Before I go asking more questions, how did you get to that point right from the start?
  
  -David
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  - Glenn Schroeder @ David Bracke on May 5, 2020 9:13 AM
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    David Bracke wrote:
    
    Hello, Glenn,
    
    So I see the very first image you have posted in your reply. You have pulled up the File Properties menu, under the Custom tab, and you have a drop-down menu in the third column. I can't get that drop-down menu to show any options at all (there is one option, and it is blank ...)
    
    Before I go asking more questions, how did you get to that point right from the start?
    
    -David
    
    That drop-down list has always been there for me without any input. I thought it was built into the software. I can edit the list in the "Property Name" column with the "Edit List" button at the top right corner of that dialog box. It might work for the other drop-down, but I haven't tried.
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    - Matt Peneguy @ Glenn Schroeder on May 5, 2020 9:21 AM
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      David,
      To add onto what Glenn's posted, once you get how to add a custom property to the part working, you may want to look at Start>SW>SW Tools>Property Tab Builder. If you set up a template, you can quickly add this property to all of your parts in an assembly from here:
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      - David Bracke @ Matt Peneguy on May 6, 2020 6:14 PM
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        Matt,
        
        Is it possible to use that feature to quickly add the same "weight" property to many unrelated parts (not together in an assembly) ?
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  - Justin Pires @ David Bracke on May 5, 2020 10:22 AM
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    David Bracke wrote:
    
    Hello, Glenn,
    
    I'm sorry it took me a while to get back to you. I've been working on a few (dozen) other projects at work ...
    
    So I see the very first image you have posted in your reply. You have pulled up the File Properties menu, under the Custom tab, and you have a drop-down menu in the third column. I can't get that drop-down menu to show any options at all (there is one option, and it is blank ...)
    
    Before I go asking more questions, how did you get to that point right from the start?
    
    -David
    In Glen's post he is in a part or assembly and the pull down references "properties.txt" Located in programdata/solidworks/solidworks(year)/Lang/(launguage)
    
    You are likely in a Drawing and I cant for the life of me find the similar "properties.txt" that the drawing file would use. It is blank for me as well and Ive always wanted a pull down with some options there.
    
    To answer your original question: In your part or assembly, Add the property weight and link it to SW MASS
    Then in the drawing, link an annotation to that property.
    $PRPSHEET:{Weight}
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    - David Bracke @ Justin Pires on May 6, 2020 6:51 PM
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      For the image in your post, you are in the Summary Information menu. How do I get there?
      
      EDIT: I have made a sheet format which contains a Note with the syntax you stated, $PRPSHEET:{Weight}. Once I have my part modeled, I create a new drawing and select my sheet format, and in theory the syntax should automatically pull the value from the solid model in question. ... In reality, the Note doesn't update, it just stays blank. I can get it to fill in the value, consistently, by playing around in the Link to Property menu. However, I can't control the rounding of the decimal places, and I am still trying to get it to update automatically. Any ideas?
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      - Hemantkumar Patel @ David Bracke on May 6, 2020 7:30 PM
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        David, "for Summary information" > all the way top there is "Option button" besides that "file properties", under file properties there is three different tab as you can see Justin's or Glenn's image > go under "Custom" tab and you will find all the "value/text expression", click and drop down manu will appear.
        Is that what you looking for???
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        David Bracke @ Hemantkumar Patel on Jul 3, 2020 4:25 PM
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        Yes - this is what I was looking for.
        
        Sorry it took me a while to reply - things are incredibly busy.
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      - Justin Pires @ David Bracke on May 7, 2020 9:45 AM
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        The "summary window" can be found by opening file properties of the part. use below picture, your button may be in a different place, maybe up by the save button.
        
        I'm not clear on where you have gone wrong so I'll try to walk you through the entire process again using pictures and a few test files. In the ZIP you will find mass-part; this part has the custom property "weight". The name is unimportant, it could be anything you want like "Bovine", the important part is that the drawing references this specific property and the property is SW-Mass.
        
        You'll next find mass-part.DRW; the drawing for this part has the annotation weight.
        which is linked to "MODEL FOUND HERE" - DRAWING VIEW SPECIFIED IN SHEET PROPERTIES - PROPERTY NAME WEIGHT.
        The "DRAWING VIEW SPECIFIED IN SHEET PROPERTIES" is a predefined view in the mass-part-template.DRWDOT named "Primary view". Allow me to explain the above: when you use this template, with ANY part, the predefined view is populated with that part and because we linked our weight property to the view it will work with any part and you can even replace the part in the view and it wont break. Unless you delete the view, then the property would look to a view that doesn't exist.
        
        To recap:
        1) add custom property to part, name it,and give it the property SW-Mass
        2) create or update your drawing template with the annotation for weight linked to either a predefined view (my preference) or DEFAULT (default will be the first view you insert into the drawing if no predefined views are present)
        3) Drink coffee and enjoy
        
        Which brings me to my next point, I'm on my first cup so if anything is unclear, Ask.
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        mass property.zip233.4 KB
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Glenn Schroeder Apr 15, 2020 3:22 PM
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Did my reply above help?
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- David Bracke @ Glenn Schroeder on Jul 3, 2020 5:06 PM
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  Hello, Glenn,
  
  My apologies, life has been incredibly busy and I had to put this on the back-burner for a while.
  
  I understand most of your explanation, and all of the recap. (Would you find it acceptable to substitute soda in step 3?)
  
  Right now, I'm working on a macro to do that (to the .SLDPRT file, add a custom property "Weight", with the expression "SW-Mass@INSERTFILENAME.SLDPRT" ) as well as select the material and change the units from metric to English. By recording my actions, the macro only reads the material selection. Do you have experience with macros / VB ?
  
  Thank you again, and sorry for the delay,
  -David
  
  EDIT: I made my own part template and drawing template to do it all. Turns out that's easier than a macro. Thank you again, Glenn.
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In a new sheet format, how can I set an automatic field that displays the mass of my solid part?

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