You need to consider what you expect to achieve with such a conversion via DXF. An assembly drawing from UG is not going to be able to export via DXF into Autocad and then re-assemble all the 3d geometry plus drawing layouts with views and associative dimensions. What is more achievable is a 2D version of the lines with a limited amount of text and no real maintainable dimensions.
By the way you wouldn't want to bring that data back into UG as part of the way you intend to work. Since the drawing will be degraded by comparison with what you had to start with you're better to maintain it using UG.
I'm afraid that whenever users ask these sorts of questions I have to ask why you want to do it. If it were up to me I would prefer to maintain the data in UG and pass on information to others in the form of a PDF file that they can view and mark up in Adobe Acrobat or similar.
dxf is only good for exporting 2D lines from a flat pattern etc, this will give you the coordinates that your laser cutter needs in order to cut the profile.
I suggest exporting your drawings as CGM files, these can then be inserted into a word document and viewed by anyone wiht MS office, or viewed directly via some free software on the internet called larrson view.
This is pretty much what I'm suggesting also. I'm referring back to a longer posting made recently which supports your comments. Since we lacked the 2D exchange license on some seats I reverted to using cgm export then import then DXF using a macro. It may sound cumbersome, but the macro takes care of most of the steps and seems to get through the conversions.
I'd like to hear from people who have had luck with the 2D exchange especially in batch mode as I can see that really working to your advantage.
As for 3D geometry via DXF it does perform a conversion, but it isn't good. If you take even a simple folded bracket comprising only planar geometry with a few radii then the DXF translation appears to create sheets from facets. IGES on the other hand manages better to take 3D geometry into Autocad, it appears that the individual flat faces are created as sheets with their original boundaries. Whether this is the fault of that way UGS does it or a limitation of DXF I can't be sure, but as you said DXF is not good as it.
We use dxf files for our cnc laser cutting machines everyday. Here is how we create the curves to export inside of NX4 modeling. We do not use drawing information to create the cnc paths for the laser machines.
1. Create a solid model of your object. We need to make sure the face that we will make the profile from is located at Z0.
2. We then change the work layer to 201 (this is required for our machines; other users may have other requirements for their machines).
3. Pick the Insert>Curve from Bodies>Extract... command (you may have to turn the command on from the customize commands menu).
4. A dialog box opens named Extract Curve. Pick edge curves> All in Face. Now pick the face of model located at Z0. The edges of all features on selected face will highlight red. Now pick OK twice and then the cancel button. The curves created will turn green.
5. Turn off all layers except the layer with the Extracted curves on.
6. We check the generated curves for splines. If any are present, we convert them to lines and arcs using the Simplify command with the delete original option selected.
7. Pick File>Export>DXF/DWG… command.
8. Select all curves on screen with Class Selection
9. Make sure the DXF option is set.
10. Specify the file name and folder location for your output file.
11. Choose Settings File button if a customized setting file is used or pick the Modify Settings to set options needed.
12. Now pick OK to start export operation.
13. Pick Ok to clear remaining open dialog window after export is completed.
14. If the curves are no longer needed, delete them and rest your work layer back to the previous layer used.
This method is used for exporting 2D curves only. We use the default green color as the laser software is not fussy on color.
As for creating the DXF or DWG drawings, we create a CGM file from Drafting first and then import that file back into the NX modeling application for export to DXF or the DWG formats.
We do not use the 2D Exchange option at all. It does not give us clean files that the laser machines can use.
Yes for 2D Profiles. Again a macro or a journal helps to automate what can otherwise become repetitive. Like you we do this quite often.
You can also adapt the technique for flat patterns if you use the sheet metal forming flattening option, (licenses permitting). This option creates curves so there's nothing to extract, and your settings will dictate what layer they'll be output on. With the macros that I had set up to do these I still put a copy temporarily onto a scratch layer in order to control the origin for DXF output. We always model in absolute and maintain the flat patterns relative to the models but DXF sent to Autocad appears more user friendly if output in the absolute XY plane with the origin at a nearby bottom left corner position. I imagine machines that accept DXF be much the same. Which is to say at least we've never had any complaints.
For drawings as a whole my take on the problem as described is that outputting curves for a 2D profile and outputting a drawing with borders views etc, would be two different requirements. That's why I'd recommend different solutions in either case.
DXFDWG-converter:
Not an option. The exported file is not a flatten 2D-drawing.
UGto2D:
This one flattens the part completely. This converter is the easiest way to create a 2D-file, however the linefont-, color- and characterfont-mapping has to be configured correctly for your application. We use PEPS-wire for programming our WEDM-machines. Linefont and color-mappings work correct; characterfont-mapping is not working. Exported text is shown in ACAD, but PEPS does not display it. Search for the right textfont is started.
Problem with the UGto2D-converter is Tc-integration: native this converter works quit well, with Tc-integration it doesn’t work (NX5.0.1.4 MP04 and also NX5.0.2.2 MP02). In NX5.0.1.4 MP05 and NX5.0.2.2 MP03 this should be fixed.
This converter can also be used very nice in cooperation with the UPM to create batch-exports.
CGM-method:
I tried also the CGM-method. Works also very nice, but is exhaustive. First you have to export a CGM, then import the CGM to a part and then export the part to DXF. The nice part of the CGM-method is that you can choose to smash text to lines and arcs: you can get a file that can be read by any software that supports DXF-files.
Disadvantage is the batch-export: to create a routine for batch-export with Tc-integration is a programmers-job.
My preference goes to the UGto2D-converter, because it’s a one time conversion and the batch-export is easy to integrate in the UPM.
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