Is this the best way to get 2D DXF for a laser cutter

[obe0009]

Hello,

Is this the best way to get 2D DXF for a laser cutter
I did creating the DXF the following method (AVI include, comment is in Dutch )
You can need tscc.exe for codec from techsmith.com.
[ul]
[li]Create new layer[/li]
[li]Extract curve from body (face option)[/li]
[li]export 2D exchange.[/li]
[li]Select the geometry[/li]
[li]Write the results to DXF.[/li]
[/ul]

Regards,

Olaf

 

[JohnRBaker]

Why are you manually extracting face curves when the File -> Export -> 2D Exchange... operation will automatically extract/project all of the visible edges and silhouette curves?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[looslib]

We used to create a flat_pattern view on layer 122, which was the 2D flat pattern outline and export just that view/layer to thge DXF for our nesting software.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[obe0009]

Hello John,

I did not know the exact function of 2D exchange. Do I get then a single curve or twice the curves because
there are two edges (top and bottom) on the solid?

Regards,

Olaf

 

[obe0009]

Hello Ben,

Thanks for the advice I will try this.

Regards,

Olaf

 

[JohnRBaker]

There's an option to exclude overlapping objects.

Note that stating with NX 8.5, '2D Exchange' no longer has an option to create DXF or DWG files. That will now be done using the new 'AutoCAD DXF/DWG Export Wizard' which includes built-in options covering both 2D and 3D formatted outputs.

BTW, if all that you're looking for is to get a 2D 'flattened' representation of the model as seen on the screen, an easier workflow might be to use the File -> Export -> CGM... function. Then just open an empty part file and import the just exported CGM file and you now have an NX file consisting of a 2D wireframe version of the model.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[frankbe]

please use NX's sheet metal functionality;

1)Convert to sheet metal
2)Create flat pattern
3)export flat pattern to either DXF or GEO
and you're done

Always 1:1 with the face up and direction you decide.

2x NX8.5 Mach Design
NX Beta Tester
1x Solid Edge ST2

 

[Toost]

Check if that other system accepts .cgm files.
Then the export is simpler/ faster. ( Cgm exports from NX are always flat.)

Regards,
Tomas

 

[obe0009]

Hello,

Thanks for your input. I made an avi for my students.
See the attachment, text and sound are in Dutch.
I don't know if it is the best or easiest way.
But I hope it is student proof.

Regards,

Olaf

 

[frankbe]

Hi Olaf,

You can make the process even quicker and more bullet proof by using the sheet metal function "export flat pattern"
In the dialog of that function you are just asked to point to the flat pattern that you want to export.

If the flat pattern definition already had an X-direction defined (which you didn't use in your video), that X-direction will also be used in the export without having to define that direction again.
In that flat pattern definition you can also define additional curves or points. That can be very useful for a laser engraving process. These engraving lines can be defined in a different colour, linetype and layer if wanted.
If believe this approach is even faster than yours.

As already mentioned you can also, very specifically, define what line types will be exported in what color and line type. That definition can be found in two places:
File - Utilities - Customer Defaults - Sheet Metal - Flat Pattern --> "Curves" and "Annotations"
Here you can define you standard. Engraving lines are called "added top and bottom geometries" BTW.

The way the flat pattern looks on your flat pattern view (also used in your draft files) can also be defined here at any time but these settings will not be remembered as your default settings.
Preferences - NX Sheet Metal - Flat Pattern Display

Hope this helps.



2x NX8.5.1.3 Mach Design
NX Beta Tester
1x Solid Edge ST2

 

[obe0009]

Hello Frankbe,

I was looking at your comments and trying to figure out how to do it,
because now we needed to do some manual nesting in an assembly and get
some engraving on the items.

But I can't find the export flat pattern menu. I can find only the export GEO Trumpf
option my NX version is NX 7.5.5.4. This is no problem because I have a working method,
but still I would like to know how you do it.

Your comment about selecting additonal geometry was a good one because we need
to do some engraving. I used 3D text to put on the solid/sheetmetal and
tried to export it with flat pattern but with no results.
This gives me a problem can you help me out with this?

Our software recognizes RGB blue 0, 0, 255 as for engraving, I believe
that colornumber 211 of NX has these properties.

Kind regards,

Olaf

 

[JohnRBaker]

In NX 7.5, there is NO option to directly 'Export' a Sheet Metal flat-pattern to a DXF file (that option was only added in NX 8.5). This means that you will need to use the normal Export -> DXF to move your flat-pattern out of NX and into a format suitable for whatever application you're using to perform the nesting.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[frankbe]

Hi John,

Export flat pattern with both DXF and GEO was introduced in NX8.0
I know because I liked it a lot

see you again in Cypress!

2x NX8.5.1.3 Mach Design
NX Beta Tester
1x Solid Edge ST2

 

[obe0009]

Hello,

I want to say thanks to all the users who gave me advice. ( It is a little bit late ).
In the end I did not use any fancy functions in NX75. I used the standard functionality in NX75.

I made curves in the part (red and blue) for engraving and cutting. See avi s. Text and speech are in dutch in the avi s.
(werkvoorbereiding_parts_01.avi and werkvoorbereiding_parts_02.avi , I had to split them due space problems with uploading)
I put them together in an assembly and create in the assembly a DXF file
(werkvoorbereiding_assembly_01.avi)

I hope this mail can contain three links to the files and not only the last.

Regards,

Olaf

 

[obe0009]

Here is werkvoorbereiding_parts_01.avi

 

[obe0009]

Here is werkvoorbereiding_assembly_01.avi