no success using DXF/DWG export in NX5
no success using DXF/DWG export in NX5
(OP)
We have been unsuccessful trying to export a .dxf or .dwg format of a NX5 drawing. We are working within Drafting and have tried numerous option combinations within the export dialog. We use NX through Teamcenter Eng., but have also tried in native. Dxf mode will produce a single view with scattered lines while dwg is either a blank view or unreadable. Yes, "All Views" is selected. Has anyone been succesful with this type of export and what settings were used? Thanks





RE: no success using DXF/DWG export in NX5
With all of that said, we are running NX 5.0.6.3. A few service packs ago the 2D exchange function started going a little nuts. Dimensions and notes would go all over the place. Siemens knows about the problem and is working on a fix for the next release. Until then, we have one person here who has several old versions of NX loaded on their machine for exporting 2D drawings.
RE: no success using DXF/DWG export in NX5
It may be able to help you.
http://www.eng-tips.com/viewthread.cfm?qid=222710
RE: no success using DXF/DWG export in NX5
1) Export the NX file to a CGM File
2) Import that CGM back into NX (Save it with a new name)
3) Export the new NX file to a DXF File
To put it bluntly, your washing out all of the items that AutoCAD will choke on and you are left with a series of curves that AutoCAD will deal with.
RE: no success using DXF/DWG export in NX5
However a lot of people report acceptable results using 2D-exchange, once you have it set up correctly.
The problem with the original question is that there is more that one way that it might be going wrong and we don't know what about the translation isn't working. Typically with assemblies people haven't their load options for the translator set to find components. A single part drawing in master model concept is an assembly so this happens a lot.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
RE: no success using DXF/DWG export in NX5
here are the steps to do the export:
- open the drawing in nx drafting mode
- go to file->export->2D Exchange...
- at advanced tab set the DXF revision to R14 (this is the best revision that works in all programs)
- at files tab set output to Modeling (not drafting) and output as to dxf or dwg extension
- then select the output directory and hit OK...
I thing that works...
Regards, Tadej
RE: no success using DXF/DWG export in NX5
Do not get me wrong, 2D-Exchange is a viable alternative - if everything is in place (correct patches, experience personnel, etc.). But more often than not - a deadline is looming, and the management does not care about data issues, just results.
RE: no success using DXF/DWG export in NX5
If they want to tinker with it then I disagree.
If the part is something as complex as a drafted plastic moulding then in most cases they really need the 3D model, and I state something to that effect on the drawings.
If it is a simple machined part or flat pattern then by all means take the 2D data and work to it. Even then I have some concerns with anyone tinkering with dimensions to arrive at results not faithful to the design intent.
Sometimes I figure the PDF is the best thing because if all you need to do is read the drawing and I know that is all that's appropriate then it can be printed out just as satisfactorily.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
RE: no success using DXF/DWG export in NX5
Siemens, please take note and make it easier to go from a solid model to a "good" 2D DXF!
RE: no success using DXF/DWG export in NX5
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: no success using DXF/DWG export in NX5
RE: no success using DXF/DWG export in NX5
That was the whole purpose of this, to provide a 2D drawing in a specific format from a 2D drawing in NX. Here, we have specific dwgs provided for customers that they will ask for electronic copies in a certain format. As far as 3D to 2D transfers, I can't recall being asked for .dxf format from 3D data.
I do have to say, the NX 2D translation method is not at all intuitive for what I presumed would be a straightforward task. Why have DXF/DWG in the export list when it seems to provide nothing of much use at all? CGM into 2Dexchange output to .dwg seems to do the job, though. Thanks again all. - CK
RE: no success using DXF/DWG export in NX5
I find that simple curves don't need 2D Exchange or the approach via CGM it is only drawings that provide the levels of complexity to do with views and fonts that you're writing about.
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum