Export Convergent Body as a STEP, IGES, Parasolid, etc.

[proxima_cygnus]

Hello everyone. So I imported a surface as an STL and used it to trim a solid body. The STL was imported as Convergent, as that was the only option that allowed me to use the Trim Body feature. The issue I'm having is that the trimmed solid body is a convergent body, which does not export as a STEP, IGES, or parasolid, which are the file formats I need for importing the geometry into my simulation. If anyone has any suggestions on what to do, please let me know. Thanks.

 

[cowski]

Try exporting as a JT file. I think STEP 242 will allow you to export faceted geometry, but it requires a special license.

www.nxjournaling.com

 

[proxima_cygnus]

There doesn't seem to be an option for importing JT files in Ansys Electronics. I also don't have the license to export as a STEP 242.

 

[Rob_N]

you might be able to rapid surface, or otherwise rebuild your imported STL into a sheet body. Then use that to trim your solid. that should stop it from becoming a convergent model.
Convergent tools are nice, but only if you stay within NX for your entire process.

 

[proxima_cygnus]

I appreciate the answers from cowski and Rob.

Unfortunately, we don't have the license for rapid surfacing.

Regarding rebuilding the STL into a sheet body, how can I go about doing that? Currently, I'm trying alternatives to the trim body method to get a solid with the desired surface shape.

Thanks.

 

[cowski]

I'd suggest using "intersection curve" on the desired section of your convergent body to get some curves from the surface of interest. You can fiddle with the "advanced curve fit" options and might even get a usable curve out of it. If not, you can use it as a reference and build your own spline on top of it. If the surface is fairly simple, you can use "swept" with one cross section and one guide curve. For more complicated surfaces, you might need to use through curves or through curve mesh.

www.nxjournaling.com

 

[Rob_N]

I agree with Cowski, that's how I've done it in the past. I don't deal with STLs much anymore. We outsource it to someone with Polywoorks or DesignX.

it's been many years...

 

[proxima_cygnus]

I appreciate your responses.

I've tried recreating the surface using intersection curves on planes and sweeping through them, however our surface is quite complex and I don't want to lose much detail. If I project the surface on say 20 planes, it takes about 15 minutes just to project the curves alone.

If there's a way to generate the surface with points in NX instead of importing the STL, asides from the Reverse Engineering features (we don't have the license), then I'd prefer to go that route. I was thinking about possibly using journals to get the job done.

Thanks.

 

[cowski]

What license do you have available?
The following commands might help: fit surface, through points, rough offset (legacy). I don't think that these require the reverse engineering license, but also don't think they are available in the mach 1 license...

"If I project the surface on say 20 planes..."

When trying to recreate a given curve or surface, the common tendency is to add dozens of control points/curves "so that we get an exact match". However, in 99% of cases, this is a mistake and will result in a curve/surface with undesired inflections that leads to endless tweaking and the false hope that "one more control curve will fix it". What you want is the minimum number of control points/curves to get the desired characteristics of the surface and then tweak the curve shapes to get the best match.

If your surface is complex, consider breaking it into multiple simpler surfaces with transitions (such as face blends) between them.

www.nxjournaling.com

 

[proxima_cygnus]

Hi Cowski,

We don't have the license for either of the features you mentioned.

Thank you for your explanation regarding control points, that's a great explanation. I'll have a tackle at it again.