Is it possible to create a sketch from 3D sectional view creo?

[Sandy1]

Hi Creo users,

I have a 3D model part and I have created a sectional view (still in part mode i.e. View- Section- X Direction).

Can I create a sketch (.sec) out of the sectional view I created above?

Your input would be appreciated.

Thank you

Sandy

[mwodarz_INNEO]

Hello Sandy.

You can create a curve from a section and project the contour (or part of it) into a sketch. And if you handle the references right, it will update the geometry right. To provide the curves from one part to another, you can use copied curves or better copy geometry. It depends on top down strategy or independent usage.

Hope that helps

Cheers

Marco

[Sandy1]

Hi Marco,

Thank you for the reply.

I will have to think about what you wrote a bit more. It does not seem to be a straight forward thing from what you wrote.

Thank you

Sandy

[Sandy1]

Hi Marco,

Ok I got the contour/profile projected on a plane. Now how do I save the projection as a sketch .sec? Googling is not helping at all. I am still in 3D part mode.

Thanks

Sandy

[LukaszMazur]

Simple. After projecting the contour, while you're still in Sketcher, select File > Save > Save a Copy and save the sketch file on disk. Do not exit the Sketcher or you'll save the copy of the model instead of the sketch.

[Sandy1]

Hi Lucas,

Thank you for the response.

1. In model tree while my cross section (XSEC0001) is activated (green diamond) and highlighted, right mouse click on it
2. From drop down menu, click Curve from Cross Section. New curve icon (Curve id 1171)will appear in model tree.
3. While the curve icon is still highlighted click on project (Model – Project (Under editing tab).
4. Project “references”, I choose “Project Chains”, under “Surfaces” I picked on which plane I want to project the curve in step 2, then accept (green tick). A project icon (Project 1) appears in the model tree.
5. From that point, how can I convert the projection (Project 1) to .SEC file. Note I was never in sketcher at any time.

See pic attached.

Thank you

Sandy

[LukaszMazur · Accepted solution]

Ah, OK. So it's a bit of misunderstanding. What I (and everybody else too, I think) meant, was that after you create section and curve from section, you create a sketch feature using the same plane as section's plane. Then, inside the sketch, use Project tool from the Sketching group to project the curve from section into the sketch.
When you do that, select File > Save As > Save a Copy and save a copy of the sketch to disk.

[Sandy1]

Thank you Lukas. 

The issue I was having with your solution is while I was in sketch mode, and using the project tool, I couldn't activate the curve that was created earlier. Even the proposed solution by Cormack87 i.e didn't do it.

What needed to do done was to "Project-> Loop" then instead of selecting curve from the model tree, just select the section individually from the 3D-model. 

Selecting the curve from the model tree should have done the same job, but seems Creo is fussy about it.

Thank you for pointing me to the right direction. Much appreciated.

Sandy

[Cormack87]

Hi Sandy, 

Assuming the plane you wish to sketch on is the same plane that is creating the x-section, could you not use the Intersect tool to create intersection curve using the plane and the body, then once a Sketch is created on the plane use Project > Loop selecting the curve generated from the Intersect?

Andrew

[Sandy1]

Thank you Cormack,

What I had to do is instead Project -> Loop and select the curve (from the model tree) , I had to select the cross section from the 3D model instead.

Thank you for your suggestion.

Sandy