Add a formula to the dimension

3D Design Volume Model
1

Hello

 

Do you know of a way to add a value related to the value of the dimension to the dimension text in the dimension text?

 

Let me explain,

 

We use aluminium profiles and templates for drilling.

On the plans I add on each drilling dimension a dimension in parenthesis which corresponds to the dimension to be used with the template.

This is just the position of the hole minus a fixed value (5.5mm in the example).

The problem is that if I change my drilling position, I have to manually change the dimension in parentheses.

 

Thank you for your help.

 

 


capture5.jpg
2

Hello

 

Yes, you must use the SolidWorks equations:

 

http://help.solidworks.com/2013/french/SolidWorks/sldworks/HIDD_EQUATION_MANAGER.htm

 

 

Where to link the value:

 

http://help.solidworks.com/2012/french/SolidWorks/sldworks/t_linking_dimension_values.htm

 

 

Just change the dimension, then scroll down the menu, and choose link value (by clicking on a dimension), or create an equation.

1 Like
3

in addition to @ Lucas' answer

Have you watched this tutorial?

http://www.lynkoa.com/tutos/3d/outil-de-cotation-dans-les-mises-en-plan

@+ ;-)

 

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4

I think that's + what he wants! (see photo)

 

 

The best thing I think would be to add an annotation attached to the desired coast. Then to link an equation, or a personal property depending on your case.

 

There you go!

 

Looking forward to it

 


cote_liee.png
5

Yes

 

If the goal is to have 2 different odds, create an equation of the type (by having created the PosHole value for example):

 

"PosHole" = "D1@Esquisse1" - 5.5

 

Where "D1@Esquisse1"  is nom_de_la_cote@nom_de_l sketch

 

Then create a custom property that takes the value of PosHole (in the 3D, in Files > Properties).

Finally, retrieve the value in the drawing in a note with:

 

$PRPSHEET:"PosHole"

 

Does it work to place it in "Quote Text"?

6

@Bart

That's my problem: But how do you link the text on the right to the value of the dimension...?

 

Thank you

7

That's why

 

Linking the text to the right is not possible to my knowledge.

 

On the other hand, you can replace this text on the right with an "annotation" that you attach to your side (put the arrow of the annotation on the side)

 

And in this annotation you put your personal property.

 

Look at the attached photo to see if that's what you want.


cote_lie.png
8

I guess your dimension in parentheses is a profile end dimension (to position your templates) and the other side, the one not in parentheses) is a construction dimension.

 

Why in your 3D model, after having positioned your machining, you don't add this "controlled" dimension (which corresponds to your dimension in brackets): see the dimension in light gray on the attached view.

Your dimension that allowed you to position your machining ("piloting" dimension) you can uncheck the box "mark the dimension to be imported on the drawing": see black dimension on the attached view.

When importing the dimensions on your drawing, you only have your dimensions to position your template.


cote.png
9

@flegendre :

it can be a solution, but in my case the holes are positioned in relation to the 3D sketch of my chassis and I don't always have a dimension in my 3D model and I add it in my plan.

In addition, I would like to have both sides: the position of the hole and the dimension of the template at the end of the profile.

 

Thank you anyway.

 

A+

10

Unfortunately, the text of a dimension is not interpreted by SW as the text of an annotation

a $PRPSHEET: "Odds" for example is not interpreted 

And I don't see a solution

 

 

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