Is there a way to show, via grabbing a variable I assume, a part's K-factor on a drawing (say in the title block) and have it update automatically if the K-factor changes?
Sorry, I was assuming you understood equations and global variables.
You have to put the global variable in the K Factor field of the sheet metal feature.
The Global Variable tells what K Factor to be in the sheet metal feature.The Custom Property reads what the value is for the Global Variable.The drawing note will link the Custom Property to the drawing.
Create a Global Variable for the K FactorCreate a Custom Property and use the syntax shown to link the global variable to the part's propertyInsert that property into your drawing.
Global Variable and Custom Property can't be named the same thing.
I just did this and it worked fine, except that, when I then changed the K-Factor, the Custom Property didn't change to match.
Where could I be going wrong?
No, I have never used a global variable before.
It works well now.
Scott, this is great.
Is it possible to include this setup in a standard startpart file, so that it is automatically populated if and when the part includes a sheet metal feature?
Ideally, I would like to have the K-Factor show up, parametrically, automatically, on any drawing of a part that includes a sheet metal feature.
Can that be done?
Create the global variable, sheet metal feature, and include the global variable into the bend allowance box. If you save this into your part template it will show up the next time you call on it.
Create a dummy base flange so the Sheet Metal feature shows up then go back and delete the base flange feature and the corresponding sketch.
>>Create a dummy base flange so the Sheet Metal feature shows up then go back and delete the base flange feature and the corresponding sketch.<<
That's the part I was struggling to figure out.
you can create a new global variable, and ether read the value for this variable to the K-factor dimension (its "D1@Sheet-Metal")
or link them backwards.
Then you can assign custom property which will read the global variable.
And on the end you just have to put a note in your sheet format and link it back to part custom property.
See the images for reference.
And I would save a "blank" part with this property as a part template.
Hope this helps.
The cut list properties callout for a sheet metal bend allowance is:
And can be used in notes added to the flat pattern. It is the cut list properties for the flat pattern, so would need to be attached to the flat view as a note. The note could be saved as a favorite, and added to views as needed.
To get to the cut list properties in general:
Right click on a drawing view of a flat pattern (must be a flat pattern), pick menu item "annotations", "cut list properties". This brings up a listing of properties as a text box. Right click on the text box, pick menu item "edit text in window" to get the following:
Bounding Box Length: $PRPWLD:"Bounding Box Length"
Bounding Box Width: $PRPWLD:"Bounding Box Width"
Sheet Metal Thickness: $PRPWLD:"Sheet Metal Thickness"
Bounding Box Area: $PRPWLD:"Bounding Box Area"
Bounding Box Area-Blank: $PRPWLD:"Bounding Box Area-Blank"
Cutting Length-Outer: $PRPWLD:"Cutting Length-Outer"
Cutting Length-Inner: $PRPWLD:"Cutting Length-Inner"
Cut Outs: $PRPWLD:"Cut Outs"
Bend Allowance: $PRPWLD:"Bend Allowance"
Bend Radius: $PRPWLD:"Bend Radius"
Surface Treatment: $PRPWLD:"Surface Treatment"
Do you know of a way to show it without having to attach a leader? Cut List Properties are greyed out unless you attach. Most drawings I see, make, or use have this information in tables like K factor so you're not hunting for the information. Do you know something different?
Also doesn't need to be a flat pattern
Thanks. This worked perfectly!
OK so the global variable part worked perfectly, but how exactly do I show in in a drawing in the form of a text string (a note)?
This is what I use....
Just saw this message tonight. Thanks, very helpful.
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