Extract a 2D section from 3D part

[plafortune]

Hi, 

I would like to extract a 2d section from a 3D part, to later export and use this 2D geometry with another program. 

My idea was to create a plane (->Model->Construct->Plane) and then "extract" of "intersect" my plane with the 3D part to create the 2D geometry but I don't find how to do it. 

Any help would be appreciated. 

Thanks

Pierre 

[TrippyLighting]

1. Create a block large enough to cut away what you don't need from the opject in quaestion.

2. Use the combine tool to perform the actual cut away.

3. Create a sketch on the sectioned surface and project the outline into the sketch.

4. then you can export the Sketch as a .dxf.

[plafortune]

Hi, 

Thank you, this is a good solution. 

I have my sketch, but I need a step or iges. 

For some reason, if I create a model containing only the sketch and save it in step or iges, the file doesn't seem to contain any geometry. 

Do you know a good way of converting the dxf into iges? 

note: I don't have autocad. 

Thanks again 

Pierre 

[TrippyLighting]

.iges and .step are Solid Model formats. You could export a very thin sliver from that 3D model.

Just follow the same procedure to cut away the other part of the model.

This would, of course still be a 3D Model.

If you could be more specific about what the desired engdresult is it would be much easier to give you advise.

[jeff_strater · Accepted solution]

A couple of things:

1. To get the section, you don't need to actually split the body.  You can just sketch on a midplane, and use Project Intersection, choose Body as the type, and select the body.  This will create a nice sketch section of the body at the position of that plane

2. You can get STEP or IGES to export this, if you turn it into a surface body.  Go to the Patch workspace, and use Boundary Patch to create a surface body of the areas of the section you want to export.  Then just export this one body.

Here is a (rather long, I apologize) screencast showing how to do this:

Jeff Strater (Fusion development)

[MattPerez314]

Instead of making solid geometry you can simply start a sketch on the plane you wish to use to cut your geometry.  Form the Sketch drop down to "Project/Include" and then select "Intersect".  You can select faces you want the sketch plane to intersect with and it will create a reference line.  This way you don't have to decimate any geometry to make it work.  Once the sketch is done simply select it from the Sketch folder, right-click and Export as DXF.  As a double check  you can also right click on the sketch and select "Slice Sketch" which will create a section view.  Depending on how complex your geometry is the slice can be a good visual check before exporting the dxf.

[MattPerez314]

Sorry, this question was open in my browser from earlier and i didnt realize Jeff had responded since then. What he said 🙂

[plafortune]

Thank you for your help!