Remove Bend Lines in Flat Pattern for DXF

[sales5N2FF]

Hi,

I'm creating DXFs to be lasercut. I'm exporting in 2010 format (earliest format the machine's software, Dr. Abe, recognizes). I can't find a way to remove the bend lines (NOT bend extents, I get that) in the drawing before exporting. I can hide them from visibility and they don't show when I preview the DXF in DWGSee, DWG True view, or import it to Inventor, but they exist when the laser operator opens them in his application.

I should also mention that I have some parts that don't have bend lines appear in the drawings, but I have no idea how or why those are different.

Thank you!

[CCarreiras]

Hi!

The faster way, select the lines and turn off the visibility.

[CCarreiras · Accepted solution]

To several views at the same time:

Select one of the Bend Lines and turn off the respective layer

[CCarreiras · Accepted solution]

To be permanent:

1. edit the layer style
2. delete the view
3.  save the file as template

[sales5N2FF]

Deselecting visibility does not work. I cannot see the lines when I open the DXF, but the program for the laser still recognizes those lines.

[sales5N2FF]

I rejoiced too soon. Sent the file over after turning off the layer and their program is still finding the line.
Thoughts?

[BDCollett]

Is the part sheet-metal and you can export from the part?

[sales5N2FF]

Yes, sheet metal part that I create a flat pattern for, insert into drawing, save as DXF.

I've attached the DXFs I can make using the suggestions I've received.

[CCarreiras · Accepted solution]

Have you tried to create the dxf from the Flat Pattern Interface (Save copy as )?

You can set up how you want to export the dxf (which layers, line type, color code, dxf year version, etc.) and save the configuration for future exports.

The final result will have only the layers you select and will be always in 1:1 scale.

This process is the standard to export flat patterns to dxf cutting machines.

[BDCollett]

As @CCarreiras said, try using this method. You have more control over the outcome. You can also use addons or iLogic to automatically generate the dxf then too.

[rhenstenburg]

Different but related:

We are looking into purchasing a laser cutting/etching machine.  Performing a Save Copy As... by right-clicking on the Flat Pattern node in the browser, one can export a DXF or DWG.

The most important aspects are as follows:

*The exported drawing is full scale

* Counterbore/Spotface/Countersink lines will be in a named layer that can be turned off

* Bend lines and Bend Extent lines are each in a named layer and can be turned off

* Laser Etched lines are in a named layer and can be distinguished from cutting lines

All good.

In the meantime, we are exporting out drawings to DWG and sending them to laser cutting vendors. 

After learning a bit about laser cutting machines, I now note that these exported IDWs:

* Are at the scale presented in the drawing file (OK, vendor can scale)

* Bend lines will appear in a named layer that can be turned off (good)

* Text, drawing border and title block can be turned off (good) BUT ...

* The part outline (for cutting) plus Counterbore, Countersink, Spotface and laser etched lines all are put into the visible layer.

This requires us to additionally process the drawing so that these non-cut items are distinguishable or deleted (tedious, error prone and undesirable).

Wouldn't it be nice ...

If we are exporting the drawing for our vendors anyway, is it possible to make:

* Etched lines export to a separate, named layer (so the machine will etch and not cut) and 

* Counterbore, countersink, spotface lines export to a separate, named layer (so they can be turned off or deleted)?

Note: Thru holes should remain part of the Visible layer so that these are cut.

Another nice thing for laser cutters:

We do a lot of pilot holes for match drilling and installing rivets.  I would love:

* Inventor having a special "Pilot Hole" feature.  The hole may appear as a small diameter hole (possibly settable) in a drawing but it is really only a location and is distinguishable from normal holes.

* These pilot holes would be exported to separate, named layer which the laser cutter can be programmed to recognize.

* Pilot holes will not be cut as round hole; rather, the machine will just perform a single pulse thru the material at that location.

Again, this would be nice to have whether exporting a flat pattern from the model file or saving an IDW as a DXF or DWG.

I am still using INV2024.  Please excuse me if some of this is handled in later versions.

[johnsonshiue]

Hi Rob,

Regarding the etching, I assume the Mark feature should fulfill your need. When exporting the Flat Pattern to DXF (from FP environment), Mark edges are exported on a separate layer.

Regarding separating hole types onto different layers, it is true that Flat Pattern DXF export does not separate hole types. But I think you may use Model States to manage the holes. For example, you may have Primary state as the all-included version. And you may create a Model State by keeping Spotface Holes only and suppressing other hole types. Then export the Flat Pattern accordingly.

Many thanks!

[rhenstenburg]

@johnsonshiue, Exporting from the flat pattern node in the browser tree of a sheet metal IPT gives ALL the desired characteristics I would want:

1) The etchings (from Mark) go to a separate, named layer (can be programmed in the laser cutter to etch, not cut)

2) Contersink, Counterbore, etc. lines go to a separate, named layer (can be shut off/deleted, as desired, so only thru holes are cut)

3) DXF is at FULL scale

My point: When exporting an IDW to DXF (or DWG), it would be nice that (1) and (2) was a feature in the resulting file.  (It is understood that any flat pattern in the IDW would be exported at the scale in the drawing; point 3 above cannot be obeyed). 

[rhenstenburg]

Forgot to mention Bend lines and bend extents.  These go into separate, named layers when exporting from the IPT.  Would like the same occurrence wheh exporting an IDW which has a flat pattern.  If the flat pattern is at FULL scale, the vendor can use it directly.

[johnsonshiue]

Hi Rob,

Many thanks for the clarification! Indeed, DXF export from an idw/dwg does not distinguish between regular component drawing views and sheet metal drawing views. There isn't an out-of-the-box workflow to do what you would like to do at the moment. I suspect iLogic might be able to help customize the workflow in this case. However, it might require in-depth knowledge of Inventor API and iLogic.

Thanks again!

[rhenstenburg]

Thanks, @johnsonshiue. I do programming with iLogic so this is a possibility but will probably not execute. 

We are moving to Vault Pro soon and can surely automate the generation of DXF's from the model file.  I was looking for a simplification for our CAD designers whereby they only have to generate one file, the DXF of the IDW drawing, to cover BOTH communication of the drawing to the laser cutter vendor and a useful flat pattern for their machine.  Looking forward to Vault Pro!