NX5 - DWG / DXF

[Simon205]

Hi, I'm having some issues trying to export 2D engineering drawings from NX to a dxf or dwg file that others could open ok. I've tried altering many of the various export options, but I'm consistently experiencing the following:

1. views showing partial geometry of components
2. views not showing part geometry at all
3. all annotations, dimensions etc... seem to come through fine
4. title blocks (which are imported patterns in NX) do not come through at all

I've tried opening the test output dwgs in NX and in Edrawings viewer just to make sure it's not an opening problem, but I get the same results with both.

Any insight appreciated.

Simon

NX 5.0.0.25

 

[hudson888]

What works is to put out a cgm then import it into an empty file and make a dxf from that. Most other methods have some hiccups. This method renders the drawing into totally dumb data but it pretty much always looks right. You can even choose to render the text to lines and arcs.

Whether any other method actually creates anything useful or not has always been something that I felt to be debatable. As I say when often this question comes up you could probably do just as well with a simple PDF if all your recipent needs to do is read the drawing or print it out.

Cheers

Hudson

 

[NilsK]

Choose the Modeling option in the Output to drop-down menu under the Export to -caption(2D Exchange options), and the drawings should come out just fine. Keep all the other options as default for the first try.

-Nils

 

[Simon205]

Hi Guys, thanks for the replies.

Hudson, exporting to a .cgm seems to flatten the drawing very well, but exporting to the dxf is where it falls down, and the final result is no geometry coming through at all
Nils, I've tried both the Export>DWG/DXF... and Export>2D Exchange options and messed around with all of the settings but can't get any useful results so far.

I'll try upgrading to a later service pack tonight to see if that solves the issue.

Cheers,


Simon

NX 5.0.0.25

 

[BOPdesigner]

Regarding 1 and 2. Using 2D Exchange, I experienced this the other day and it was because all my assembly components were not in the same drawing folder (native mode). I know, I know, why the heck would that matter? The translation tool actually rereads all the open components as part of the exchange process. So, even if you have your assembly load options set to search folders or something, the Exchange tool doesn't read that. If this situation applies to you, I can dig up the string variable you need to change at work tomorrow.

 

[Dave K]

Simon,

Do you happen to be running on Vista64? I just got a .dll patch, for dxf/dwg issues with the 64bit version of NX5.


-Dave
Everything should be designed as simple as possible, but not simpler.

 

[Simon205]

Thanks for all the replies.

Right the problem has been solved, but neither myself or the guys from NX support know why!

After trying lots of different options with the DXF/DWG Export & 2D Exchange options, the following worked:

File>Options>Assembly Load Options>.........changing the 'load' option from 'From Search Folders' to 'From Folder', exporting something by 2D Exchange, then changing the option back to 'From Search Folders'.

And Voila!

Thanks for the help

 

[hudson888]

The same thing is for STEP. Had you mentioned that it was an assembly or even the words master model in connection with your drawing that might have alerted if not me then somebody to what the problem was. It is a good one to remember for the future.

Cheers

Hudson

 

[BOPdesigner]

When you use 2D Exchange with search folders you can save your assembly load options (ex: load_options.def) and then in your ugto2d.def file you point to this file under ASSEM_OPTIONS = . I suspect it would be the same for the dxfdwg export but in the dxfdwg.def (and ugstep20X.def) file, the variable names are different. I am not sure you if you would use UGI_LOAD_OPTION or UGI_SEARCH_DIRS. I can't find information on either of these variables when I search the online documentation.

 

[DavidTolsma]

Upgrade NX to at least a dot release. 5.0.0.25 is the initial release. 5.0.4 would be a good choice. The latest the better. Don't bother with any MPs unless they fix a specific problem related to DXF that you are running and have no option to upgrade.

-Dave Tolsma
Tolsnet LLC

http://groups.google.com/group/NX_CAX/

http://groups.google.com/group/plm-exchange/