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Copy a cross section of a body to a new part

Experimenter
Experimenter

I have an assembly that was made from bodies in the concept stage which is comprised of several revolved bodies. The whole assembly is made of one component so the "assembly" is not properly assembled of separate components. I need to extract the cross section of each body and place it in a new part, and then revolve it. From there I will make the complete assembly with the individual parts as components. How can I extract a cross section of a body without a sketch to work from?

3 REPLIES

Re: Copy a cross section of a body to a new part

Siemens Valued Contributor Siemens Valued Contributor
Siemens Valued Contributor

Hi Corbin,

 

you could've done this very easily in NX10 / NX11, there is a new functionality w/in NX, it is NX Layout and Convert to 3D, NX will automatically convert all section geometries, or sketches into 3D components.

 

With that being said (hopefully you and your company will consider moving to NX11).

 

In NX8.5, this is what i would do

1. Create section curves of all 3D geometries

2. Use WAVE link of geometries (or file export part) of each of 3d sectioned

3. create a new assembly file and add each of components

 

HTH

 

regards

 

Sam

Sam Kuan

Re: Copy a cross section of a body to a new part

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @Corbin,

How can I extract a cross section of a body without a sketch to work from?

Place a Datum Plane through the axis of the revolved body and then use the Section command to create your section curves (you can build the datum on-the-fly with the Section command).  Dialog steps are to select the object (revolved body) and the section Plane.

Is there a reason you're not using the top-down assembly creation method (Assemblies > Components > Create New Component) and just pushing these revolved bodies down into their components on-the-fly? 

 

@SamKuan - does your solution require an additional "Layout" license?

 

Regards, Ben

Re: Copy a cross section of a body to a new part

Honored Contributor
Honored Contributor

If you have a file with various bodies that you want to turn into components, the easiest way to do so is with the "create new" command on the assembly toolbar (as mentioned by @BenBroad). Let's say that you have a solid body in your file that you want to turn into a component. This command allows you to select the solid and specify a new part file; it will move the solid (and all geometry used to create it) into the new file and add it as a component to the original file. Repeat for other bodies that you want to turn into components.