Project a sketch onto another part in an assembly

3D Design Volume Model
1

Hi all

 

A small question that must have already been asked: how can I project the sketch belonging to one part, on another part of the assembly to be able to reuse it?

 

In p.j: I want to project the blue surface on the back plate keeping all the holes, but obviously the projection is only done on the external surface and not the holes!!!!

 

Thank you


a.png
2

Hello

Several solutions:

1) Create a block: http://goo.gl/MxRIEA

2) Copy the sketch (with CTRL C and CTRL V) if it exists as it is in the room, then paste it into the other room.

3) Convert entities to a new sketch in the assembly: http://goo.gl/LcHqCM

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3

Hello

Place yourself in your assembly, edit the part where you want to copy the sketch. Select the sketch of the other part in the Feature Manager (tree) + CTRL the face of the edited part (or the plane) where you want to paste the sketch in question.

Once the 2 elements are selected (sketch + plane/face), press Insert/Derived Sketch.

There you go!

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4

Indeed, when I convert the entities (in the "chain" selection) I manage to project the sketches, but I wanted to do it in one go by projecting the face that contains the holes in order to save time...

I think it's heavy

5

If you want something quick, try the proposed derivative sketch solution. It takes 5 seconds! :)

6

And projecting entities in a "loop" doesn't exist on SW? it takes the entire contour of the selected surface

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7

You can convert entities by clicking each face, it will be much faster! SolidWorks will convert all entities on this face(s): outer and inner contours (i.e. holes)

8

@ Benoit:

Thank you, your solution works by selecting one or more sketches but doesn't work if you select a shot on which there are several sketches that you want to project...

@PL: no it doesn't work, it only projects the outer contour

 

Thank you anyway

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9
Otherwise make a rectangle with the mouse which will select all the sketches of the part, convert them, then delete the ones that are useless. This will probably be the quickest solution.
10

So place your sketch plane running through the volume of the crown and do Tools/Sketch Tools/Intersect Curve. In the window provided, select the crown body (and not the faces) in the Feature Manager, then confirm. You'll get the whole section!

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11

@ Benoit:

 

bravo your solution works, it's a bit laborious (it adds an operation) but hey it works...

 

Thank you

1 Like