Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

NX10 and NX11 Export Flat Pattern as DXF

Gears Legend Gears Legend
Gears Legend

Hi guys,

 

did anyone of you notice that the flat pattern export as DXF doesn't always orientates the view correctly?

The Flat Pattern View itself is correct however. The Flat Pattern Export to GEO is also correct. I remember that Thomas talked about it during our last call.

I never noticed this before because in 99% of the cases we only use the Trumpf GEO export.

 

BTW I just filed IR8316662 on this subject.

 

I attached the NX10 and DXF file to have a look at.

 

Thanks

Huysmans Metalen n.v.
2x NX 11.0.2.7 Mach Designer
on Win7 64bit
NX Beta Tester with focus on Sheet Metal
Command Finder is your friend
8 REPLIES

Re: NX10 and NX11 Export Flat Pattern as DXF

Creator
Creator

To demonstrate I've created a simple example.

 

I started with a Triangle Tab and attached a standard flange with a rectangular web.

A Flat Pattern is added, the Triangle was selected as reference face. No extra Orientation was used during FP command.

The vector of the triangle face shows to Y of the bent 3D model CSYS.

s1.pngs1 

The FP in Model Views looks correct. NX "knows" here where the Z direction of the FP is. It's not the Z-vector of CSYS of the 3D Model. Nothing was manually turned for the screenshot.

s2.pngFP Model View  

Let's look in the FP view in the drawing. NX "knows" here too where the Z direction of the FP is. I think it's the same algorithm behind. Again: The Z-direction was not manually adjusted.

s3.pngFP Drafting View 

I've exported the FP to DXF

s4.pngFP Exp Dialog 

Little additional critic here: When I have only one FP feature, why do I have to choose one? I think, at the moment 99% our SB Models have only one FP. For me it's a unnecessary step. I would expect here in that case, the "* Select Flat Pattern Feature" is automatically "green".

 

 

During the command execution I see for a moment switching to the view how the DXF export looks like. Here I would wish that the "picture" is shown to the user "So looks the Flatpattern Export export", and after pressing OK-button the real DXF export will start. So it is done in "our" customer export. I could imagine, this behaviour (show the export or not) could be set in Customer Defaults or Preferences. The FP DXF export can look different to the FP view in NX – depending on the line types selected in the dialog (FP Geometry Types).

 

Next thing what we have implemented in our custom export is the option to mirror the FP in DXF. This could be useful for other companies too and should be part of the "Export FP" dialog.

 

The DXF file shows the FP from the side, the default view is Top, but Front or Back show the FP in Z-direction. The DXF refers to Z vector of the 3D Model, which is a bit inappropriate here. I think it should be no big issue for the programmers to change this to the alignment of the flatpattern. The reference to the Z vector of 3D Model makes from my point of view no sense, maybe it was just done by accident.

5.pngDXF from side

 

Yes, I know I could have used the rectangular face as reference during FP command or could have used the Orientation option. Please keep in mind in practice (at least in our company) there are a many different people involved. The creation of the part, the creation of the FP, the creation of the drawing, the creation of the DXF and the usage of the DXF is not done by one single person. Even if it would be the case, there can be something forgot or done wrong.

6.png (FP DXF with correct Z)

 

About the suggestion introducing a Orient option in the FP Export dialog: Nothing against it, but this option should not be needed to have the Z vector of the FP fixed. The Z vector of FP is already known and should be used for the DXF too. This Orient dialog should be only be there to turn the FP around the already known Z-axis.

At the moment we don't need to turn the DXF very often. The rotation for nesting for the punch nibble or laser cutting etc. is done with the DXFs by another guy in another system.

 

About DXF/GEO export into Teamcenter: I support this idea. Please make the creation of the names configurable in customer defaults. For us it would be sufficient or let's say it's mandory that this can be done the admin centrally – maybe in other companies the end user will or have to influence this.

 

DXF Export to native in managed mode: This is our current standard situation. Let's assume the Item is "1234" and the current revision is "A1". The NX export will name the DXF "1234.dxf", our custom export will name it "1234_A1.dxf". Maybe I missed it, but I don't find the option to configure the name. If there are more FPs, the FP name or the number of it should be configurable too, something like "1234_A1_FP01.dxf".

 

For automation things it would be nice to have a command line mode. There should be a control which line types are included or not. 

 

I made a strange observation: When I have more FPs in the part the size of the DXF is growing. I assume it's more exported than needed. But I'm not 100% sure, maybe this should be investigated.

 

 

Summary

Our "demand":

  • Turn the FP DXF to the "correct" FP Z axis (which is already known) – without additional need to select the "Orient" option.

 

additional suggestions:

  • no need to select the FP feature, if there is only one
  • an option to mirror the DXF (only the DXF, not the FP in the NX-part)
  • configurable: display the lines how they will be exported, before the export
  • an option to influence the angle of the DXF, around the known Z axis
  • make the export name fully configurable:
    • for Situations: prt in TC -> dxf in TC, prt in TC -> dxf in native, part in native -> dxf in native
    • the name setting for all situations (see above) should be independend from each other
    • options for the string should include Item, Item Revison, FP name, FP sequence (and part name if native mode) – more ideas?
  • command line mode

 

 

Yes, it's a shame, we have different locations, product areas, departments etc., but I've seen nowhere GEO used, only DXF. On the other side: Never touch a running system.

 

If needed, I can open an ER for my suggestions.

Example files and original text is attached.

Re: NX10 and NX11 Export Flat Pattern as DXF

Creator
Creator

Hi Frank,

 

I adjusted your model. Created a new Csys, Z is 90° to the ring face, oriented the part to the new CSYS. I didn't have to re-apply the FP.

Seen too late, your part is NX 10, did it with NX 11, made a screenshot.

 

Gruß

Thomas

 

PS: had to zip prt and dxf

Re: NX10 and NX11 Export Flat Pattern as DXF

Gears Legend Gears Legend
Gears Legend

Hallo Thomas,

 

Now that I've read your explanation, I strongly believe that something is broken in NX10. The DXF Flat Pattern Export to DXF has always worked in NX9.

But I do remember that I was broken in NX7 and in the beginning of NX7.5.

 

So what you're asking for is NOT an ER but an IR.

If we would use the DXF instead of the GEO, this issue would be a SHOW STOPPER. I remember back with NX7.5 (when there was no GEO export option yet) we didn't use NX at all for that very reason. We had to continue using Solid Edge. So now today, per coincidence, I found out it's broken again.

 

So please to development; fix this. This is important.

 

I also now understand your question during the call; I never realised it was broken in NX10.

Huysmans Metalen n.v.
2x NX 11.0.2.7 Mach Designer
on Win7 64bit
NX Beta Tester with focus on Sheet Metal
Command Finder is your friend

Re: NX10 and NX11 Export Flat Pattern as DXF

Gears Legend Gears Legend
Gears Legend

Little additional critic here: When I have only one FP feature, why do I have to choose one? I think, at the moment 99% our SB Models have only one FP. For me it's a unnecessary step. I would expect here in that case, the "* Select Flat Pattern Feature" is automatically "green".

 

Very good comment Smiley Wink

Huysmans Metalen n.v.
2x NX 11.0.2.7 Mach Designer
on Win7 64bit
NX Beta Tester with focus on Sheet Metal
Command Finder is your friend

Re: NX10 and NX11 Export Flat Pattern as DXF

Gears Legend Gears Legend
Gears Legend

Hi Thomas, hi all,

 

I just noticed that the error occurs when you DON'T select an edge for an orientation.

In my example I could not pick a valid edge because the geometry contained nothing but circles.

 

Still the GEO export does it good, but the DXF export fails.

So still an IR in my view.

The problems that we had with NX7.5 way back were also happening with valid edges being selected.

So the problem we see here seems related but is not exactly the same.

 

My suggestion is that you always select an orientation edge when possible. That is how we work.

When the IR is solved you will have no more worries about the batch processing of DXF exports.

Huysmans Metalen n.v.
2x NX 11.0.2.7 Mach Designer
on Win7 64bit
NX Beta Tester with focus on Sheet Metal
Command Finder is your friend

Re: NX10 and NX11 Export Flat Pattern as DXF

Siemens Phenom Siemens Phenom
Siemens Phenom

Good discussion here.

 

Thanks for the information and analysis.  I have requested development take a look at this and orientation of DXF output should be an IR.

 

I like the idea of DXF preview, we should have an ER for that.

 

I also agree that if only one flat pattern exists in the work part, then it should be inferred automatically.  That also is an ER.

 

I'll keep you posted on the response.

 

thanks,

Dave

Re: NX10 and NX11 Export Flat Pattern as DXF

Creator
Creator

I opened some IRs for the topics

7850490 main ticket intended to become a PR

and 7850498, 7850501, 7850507, 7850510, 7850517, 7850528 intended as ERs

 

Re: NX10 and NX11 Export Flat Pattern as DXF

PLM World Member Genius PLM World Member Genius
PLM World Member Genius

Dave,

I'm seeing all the same issues as Thomas/Frank using that workflow. But since we do select orientation like Frank, it's not as big of an issue but the bug does exist.

 

BTW, has there ever been any discussion as to NX automating the of exporting DXF's? From what I have heard talking to people, everyone seems to be forced to write their own custom code to accomplish a task that we all have to perform. Primarily generate .dxf's from NX flat patterns in order to pass that geometry/data onto 3rd party CAM software or vendors.

 

I myself am getting ready to have someone write software to accomplish this and it all seems to be redundant. 

 

Best Regards,

Ryan

--
Ryan Gudorf
CAD/CAM Supervisor
Budde Sheet Metal Works, Inc.
Windows 7 Professional x64 SP1
Solid Edge V20
NX11.0.1
TC10.1.5 32 GB RAM, nVIDIA Quadro K4200
Highlighted

NX10 and NX11 Export Flat Pattern as DXF

Gears Legend Gears Legend
Gears Legend

Hi guys,

 

did anyone of you notice that the flat pattern export as DXF doesn't always orientates the view correctly?

The Flat Pattern View itself is correct however. The Flat Pattern Export to GEO is also correct. I remember that Thomas talked about it during our last call.

I never noticed this before because in 99% of the cases we only use the Trumpf GEO export.

 

BTW I just filed IR8316662 on this subject.

 

I attached the NX10 and DXF file to have a look at.

 

Thanks

Huysmans Metalen n.v.
2x NX 11.0.2.7 Mach Designer
on Win7 64bit
NX Beta Tester with focus on Sheet Metal
Command Finder is your friend
NX Sheet Metal
NX Sheet Metal

This group is dedicated to the discussion of Sheet Metal in NX.

Members (80)