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Find Coordinates of 2D cross section of 3D part

AA_10386650
3-Visitor

Find Coordinates of 2D cross section of 3D part

Hi everyone, I have some 3D parts (an image of one is attached) and I was wondering if I can export the coordinates of the points making up a 2D cross section of my shape at various Z lengths (because the shape is extruded in the Z direction). for example my extrusion in Z is 10mm and i would like to get the points that make up the perimeter at Z=5mm and Z=2mm. I hope this is clear, I intend to use this coordinates in matlab (a programming software)

AA_10386650_0-1661173894771.png

 

4 REPLIES 4

Create planar sections at the desired Z values and export the section curves. 2D dxf format for the entities is probably the best option. You will then need an interpreter for MATLAB to read the DXF format.

 

In the model you generate the section curves by intersecting a plane at the z offset with the solid body of interest (Creo7+). If you are in an earlier Creo build you will need to intersect the solid part geometry when selecting during intersection.

 

 You can then export this closed curve using any csys in the model as an origin for the export.

 

Example of planar intersect feature (blue curve) with a solid body.

tbraxton_0-1661186383890.png

 

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric

Thank you @tbraxton, could you please aid me on how to export a section curve. Because when I created a section at the desired Z offset I can still see the extrusion up to Z and I cant see a 2D section like the one you have.


@AA_10386650 wrote:

Thank you @tbraxton, could you please aid me on how to export a section curve. Because when I created a section at the desired Z offset I can still see the extrusion up to Z and I cant see a 2D section like the one you have.


Hi,

I can only think of the following solution.

  • create new assembly
  • assemble your part to default position
  • create x-section in assembly
  • create curve from x-section
  • hide part (only curve is displayed)
  • create new drawing
  • place assembly view (set its display state as Wireframe, Hidden or No Hidden
  • export DXF from drawing

 


Martin Hanák

What version of Creo are you working in? I am not clear on your last question, have you successfully created a curve by intersection of a plane with your solid body in your model? Assuming you only have one body in your model, convert it to a construction body. Construction bodies can be excluded in export profiles.

 

Creo can only export 2D dxf from a drawing so if that is the file format you want to use you must create a drawing with your curves in a drawing view(s).

 

You can export the curves as STEP from a 3D model and use the csys of choice for the export.

To set a construction body RMB on the body in the model tree and select this option:

tbraxton_1-1661253533105.png

 

 

The option to exclude construction bodies in an export profile is shown here.

 

tbraxton_0-1661253443441.png

 

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
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