Insert the number of Solidworks sheet metal plies

3D Design Volume Model
1

Hi all

does anyone know how to retrieve the number of plies of a SW2015 sheet metal part (the equation being in the properties of the welded parts list),

in order to see this number appear in a name of an assembly where this part is located?


plis_sw.jpg
2

Either add a column and bind the number of bends property.

 

Either add a note and do the same, link the note or column to the personal property

here "SW-*plis@@... etc.)

 

See image.


plis.png
3

By creating a custom property that calls sw-plis@@@sheet<1>@piece1.sldprt?

This property will then be visible in the nomenclature, but there must not be several bodies in the part.

4

This image may be more understandable.

-right-click to add a column

- double click on the top of the column to select the source

- Select properties from the list of welded parts

- choose "Folds"

 

 


plis_bis.png
5

in fact on a drawing of the part, no problem, I retrieve the data from the list of welded parts, On the other hand in the drawing of the Assembly, I create a classic nomenclature or I add a column with the custom property of the part, but even if I choose PLIS, they don't appear!


plis_sw-2.jpg
6
I believe that this is only possible by adding an annotation related to the part.
7

Failed, I tested my idea: it doesn't work, I can't link a sheet metal prop to another prop.

And in an asm nomenclature, it does offer me the "PLIS" prop but it remains empty!

8
This is possible by linking an annotation to the piece see here http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_SELECT_PROPERTY.htm

And you have to choose "Component to which the annotation is attached"

1 Like
9

Logically, if you are in an assembly, Sw takes over the ownership of the assembly.

 

To do this, I'll insert my related part out of my sheet, I insert my nomenclature by clicking on my part out of the sheet so that the table is linked. Then the rest follows.

 

But logically, with the right formula, it should be possible, as Lucas said.

1 Like
10

What if we put the bill of materials for the assembly, and on the folds box to the line corresponding to the part we insert a note by linking the property Folds?

11

and breaking down the nomenclature 

Decomposition of a sub-assembly or welded construction in BOMs

You can decompose components of subassemblies or welded constructions into a BOM.

To break down one or more subassemblies or welded parts in a BOM:

  1. Click the left side of the BOM table to display the Assembly Structure column in the BOM, if it is hidden.

     

  2. Right-click one or more selected cells in the Assembly Structure column that contains a set of subassemblies or welded parts.

     

  3. Select Breakdown.


     

    Modified objects are marked.

It should work, right?

@+ 

12

In fact, when we put a bubble on the part, we can choose to bind the bubble to the properties of the welded parts list of Part1!

on the other hand, if I paste the note ($PRP:"Folds")  in the nomenclature box, it doesn't work.

we see in the bubble the number of folds, but not in the Nomenclature.

If we force the BOM box, the welded part list is greyed out (not accessible).


plis_sw-4.jpg
13

error the bubble formula is $PRPWLD: "Folds"

but it doesn't change anything!

1 Like
14

If your note is linked to the component to which the annotation is attached, there is no logical problem.

15

I insert my note,

 

I check the box Component to which the annotation is attached, I click on property of the list of welded parts

 

I choose Plis and that's it

 

Then if I want my note to be in a box, I remove the arrows and I put the note in my nomenclature.


note.png
16

To remove the arrow see image.


flechage.png
17

So as I said before:

Possible in an annotation linked to the document, but not possible in the nomenclature...