Auto Tolerance in Drawing

3D Design Volume Model
1

Hello, I would like to know if it is possible to transfer the tolerances I have put in the room automatically into a drawing. I don't know if I'm clear, but I wish I didn't have to re-type each tolerance one by one.

Thank you for your answers

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2

Hello

You have to use the objects in the model to insert the dimensions in the drawing: the black ones are in 3D, while the gray dimensions are only in the drawing.

For more information, here is a short video:

https://www.youtube.com/watch?v=YHPoK6zKxsA

And the corresponding help pages:

http://help.solidworks.com/2016/French/SolidWorks/sldworks/c_insert_model_items.htm

http://help.solidworks.com/2016/French/SolidWorks/sldworks/HIDD_DVE_INSERT_MODEL_ITEMS.htm

 

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3

Thank you for your answer, the problem is that I've already tried and the sides that interest me are in a design sketch, and the objects of the model can't take them into account.

 

4

Hello, what software is it and which version??? Thanks in advance

 

Kind regards

5

This is Solidworks 2014

6

In the object of the model, check that in the dimension you have the option Marked for drawing and not marked for drawing enabled (button pressed)

7

Hello

Yes, it is possible; Here's how to do it... But you have to be super CAREFUL with this function... If you double click on it in the MEP and change the dimension, it's the part that will move because these are the CONSTRUCTION dimensions...


report_de_cote_de_piece_vers_mep.docx
8

If the dimensions are only in a sketch but not in a function, this trick works:

when you are in the insertion of the objects of the model, you press "C" (the key on the keyboard) and it displays the tree, which you have to expand to get to the sketch you want! And by clicking on this sketch, the dimensions are going to appear in the drawing.

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9

Hello

Unfortunately this doesn't work every time with solidsworks 2014, you have to make sure that your sketch plan corresponds to the drawing view where you want to show your dimensions.

Example: in a revolution function, if your sketch is in the front plane and your view is on the side plane, then the dimensions will not necessarily appear.

For my part, after multiple attempts, we gave up on showing the dimensions of the 3D in the drawing.

Kind regards

Gilles

10

I'm also under sw2014 and I get the ribs on all my not too complicated parts without any problems.

11

Is it the SP5 version?
Can we see it in the menu?  > "by the way".

If it's not SP5, you absolutely have to do the update which coprfixes many bugs.

12

A survey made by alain.erp that goes in the direction of your question.

http://www.lynkoa.com/forum/mise-en-plan/cotation-des-mep-par-objet-du-modele-solidworks

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13

PL is right for the C key when we are in the objects of the model. You can choose which sketches to show.

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14

Hello @Bendix,

To complete what was said previously about the driving dimensions from the Model Objects, to correctly retrieve the dimensions of the 3D, you must first arrange your annotation views correctly.

That is to say, move in these annotation views the dimensions you want to appear (for example, a width dimension on the top view rather than on the front view).

After that, the drawing views are as you want them to be.

Note: Annotation views are with (A) in front.

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