Probably not seaching the terms that NX uses. New to NX, but it has been a very straight forward element of Solidworks, Pro/E-Creo, and Fusion360 but cant really figure it out in NX.
What I need to do:
I have a part file that I need to emboss a fairly detailed logo image and font. I have the native Illustrator as well as the ability to export it as a dxf/dwg if need be. I did manage to import a dxf vervion and get it scaled, but there was no options on what plane/face to orient it to. Also the surface it needs to be embossed onto is a complex surface so not a flat face. What is the propper procedure/work flow for doing this? I cannot find anything in the selfpaced learning and only online tasks I can find are for putting simple dxf engineering drawings into a drawing files.
I am sorry that it is not so straightforward, but it is possible.
When you import a DXF (file--> import) into the workpart there are potential unit issues. If you know what units you write the the DXf then you can choose the correct unit on import. You can also read in the DXF file it self (it is a text file) what the units are.
The curves will be placed on the absolute origin of the part. From there you will have to move them to where you want them. The tool to consider for this is Move Object (shortcut CTRL+T).
Scale curve might also be useful, make sure you toggle of "Associative" in the feature group so you do not get a feature.
Once your curves are placed and scaled then you can emboss your body them using the curves and the Emboss tool.
An alternative workflow (if you do not have too many curves):
After importing the curves, create a sketch on the X-Y plane and add the curves to it (using Add Curves when the sketch is active). This will make them one collection contained in a feature that can easily be selected. Now create a datum CSYS where you want the curves and reattach the sketch to the new CSYS. Now you can edit the CSYS and move the cures around to fine tune the position.