Show a note in SW drawing for area of the selected surface?

2D plans Layout
1

Is it possible to display a note in a SolidWorks drawing that gives the area (m² for example) measurement of the selected surface ("pointed" by the note)?

 

SolidWorks drawing

automatic note which gives the measurement = area (m² for example) of the selected surface ("pointed" by the note)

2

Hello

We can draw inspiration from the answers given here:

http://www.lynkoa.com/forum/3d/comment-peux-t-calculer-une-surface-de-peinture-sur-un-assemblage

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In my opinion the best solution is to write it by hand, I don't believe there are any automatic solutions for this.

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Otherwise, see also this thread, in particular John Burrill's  reply 23 August 2013:

https://forum.solidworks.com/message/377904#377904

But it's not that simple:

Make a configuration that's just the face that you want to measure the surface area of. To do that, create a new configuration, use the 'offset surface' toolbar with a distance of 0 to clone the surface you want to report the area on.  Create a delete body feature and select the solid bodies of your part, leaving the surface offset behind. 

Configure these features so that they're suppressed in all but the new configuration

Create and link a custom property to surface area in this configuration

If the note is is in the title-block, insert a drawing view of the part in it's surface area configuration and hide it.  Set the sheet to look at the new view.

If it's not, insert a view of the surface-area configuration, drag it off the sheet, create a note tagged to that view and drag it back onto the sheet.  You might want to lock the view so that you don't inadvertantly reposition the note.

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Otherwise, you have to use the equations, if the dimensions correspond to the width and length then it's easy.

Then create a custom property that sets the result of the equation is put it in a our in the drawing.

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Hello

Solution found by @PL. in one of my questions:

http://www.lynkoa.com/forum/cao/propriete-de-superficie

@+

 

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  1. In your room, you create an equation (in the example below the variable is called "surface_b"

NOTE: in my example above, I want a rounded result that's why the equation is as follows: = round ( "D2@Esquisse2" * "D1@Esquisse2" )

  1. In the custom properties of your part, you create a property to which you assign the previously created variable.

  1. In your drawing, you create a note that you link to the custom property of your room

And that's it.

 

The only thing I don't know how to do is put the units (automatically).

1 Like
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@Coyote: This was the question I was looking for, but without success!!

I can't wait for the search on Lynkoa to be improved...

To create a note, you need to create the property using the small program below:

So as stated in SPR 633058, linking a sensor to a property is not possible. One solution proposed in this message is to install a small add-on:

https://forum.solidworks.com/message/490783#490783

1 Like
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Too bad Dassault Systèmes hasn't developed this function.. it seems so obvious to do.

Thank you for your answers. But these didn't solve my problem.

I tried the macro area tracker add-in but it doesn't work because I'm still running with SW2014. I think that could be a good solution.

The solution with equations is too long to set up, especially with any shapes. So it's quicker to copy-paste the info to "measure".