Inventor to Burn Table DXF Errors

[Cadmanto]

The method I use to create DXF files for the burn table has worked at my past job and outside vendors.  For some reason at my current location I cannot get these DXF files to load properly in the burn station.  We are using a Lincoln Electric Phantom II.

Getting the attached error message.  Contacting Lincoln electric they get the same error.

The first go around there was an error message indicating something to do with the layers.  So I turned off all of the layers except for the geometry layer.  That issue went away, now the tech support for Lincoln is saying I have open contours.  Not sure how that is possible seeing it is a clean model with a front view.

The weird thing is if I take the part and have my coworker open it in Solidworks and he exports it, it works.

Any thoughts?

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Mark.Lancaster]

@Cadmanto

I was helping someone the other day and their laser cutter was stopping and starting at each end point like it had open profiles..   I suspected the DXF was bad for that given part since other parts would cut fine.  I told the end user to open the DXF directly in AutoCAD and see if it was water tight (like end points may not match perfectly and thus its not water tight.)    Anyhow a thought.

[Cadmanto]

Thanks Mark.  I will try this as an experiment, but my confusion comes in how does a tight model export to DXF and become open?

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Mark.Lancaster]

@Cadmanto

I never heard back from the other person I was assisting but all other parts worked fine so I was offering that as a starting point for that given part design..   It may be fine..

[kelly.young]

Hello @Cadmanto if you change the setting for .dxf to the oldest one does it work better?

In the past I had issues with my plasma output and using the AutoCAD R12 version produced the best results.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Cadmanto]

Thanks Kelly for your suggestion.  As per the images below, I did try what you said.  Same error message on the burn machine.

Now, what is interesting is, base on the error message and what the tech at Lincoln said and Mark, I imported the Inventor DXF into Autocad and and redrew just the straight lines.  The image below shows what came up on the burn machine.

As you can see, the only thing that came through are the lines I redrew.  The holes and fillets did not.  I can't help but think there is a setting somehow that I am missing.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[kelly.young · Accepted solution]

@Cadmanto I renamed the layer (removed the parentheses in case it doesn't like them), set the linetype to default, purged all other items. 

You can also try to change it to the 0 Layer and see if that makes it happier. I used an old 3-1/2 floppy water jet that wouldn't read correctly unless it was set to zero. Found out the hard way when it cut a full sheet in half mid way through the run. 

Try the attachments and see if they work any better. Is there any Event Log showing anything fishy? 

Are there any settings in the Torchmate software that set the import line options?

AutoCAD Troubleshooting in Version 5

The Internet said there might be a .dll file that needs to be updated in the Torchmate software?

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Cadmanto]

Thanks Kelly.  I will get back to this.  Just got slammed, so no time currently to do this.

I do want to test and verify what you are suggesting.  I will let you know.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Cris-Ideas]

Hi

from the image it seems clear that all splines are missing for some reason.

@kelly.youngWas there any change in handling splines on export?

Cris.

[Frederick_Law]

Your DXF has 2 layers: 0, Visible (ANSI).

All entities are in Visible (ANSI).

The error you show indicate the software is importing layer: CUT, NOKREFCUT, SCRIBE, PUNCH, PLOT, 0.

Add 'Visible (ANSI)" to the list.

Or move everything to 0.

Solidworks export geometry to 0.

If adding 'Visible (ANSI)' to the list doesn't work, You can rename "Visible (ANSI)" to "0" in Style Manager.

[Cadmanto]

@kelly.young , I am back on this.  Sorry it took so long to get back to this.

In the interim between now and the last time we chatted, I have been recreating the dxf files in a 2D software program and saving them out as a 2013 ASCII dxf file.  This will read in the  burn table.

Unfortunately this can be time consuming.  I am still looking for a way to directly export out of Inventor to dxf that the burn table can read.

I will download your dxf files and let you know how they worked.   But, this still involves an extra step in creating the perfect dxf.  My last job had a burn table and I am doing the same process here as there.  Placing a plane view on to a blank drawing sheet with no border or title block.

Truthfully, I have never used layers while using Inventor or any other 3D modeling software.

I am attaching the latest dxf I tried yet again (which still errored) along with a picture of the error code.  I have been in contact with the burn table manufacturer and they are getting the same error.

Now, with that said, they mentioned to me that they have seen some 3D modeling software's leave open ended intersections that will still allow the software to extrude features.  I personally have never heard this with any 3D software.  So they are asking me to ask you this question;  "What is the tolerance for lines being joined?"

@kelly.young as an update, I tried both of the files you attached in this thread and from the attachments, you can see one was successful and the other failed.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Cadmanto]

@kelly.young

Here are the other attachments.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Frederick_Law]

Inventor export line with ends connected.

Solid-not-works by default export dwg/dxf with ends NOT connected.

Burn table software usually have setting to connect end point if they're within a set tolerance.

[Cadmanto]

It is really interesting you say that.  We have SW here too.  If I export out any part as a step file, I can import model into SW and export directly the model into a DXF file without having to create any drawing.

Never knew about the ends not connected facet.  I guess this falls under the "Close enough" rule when it comes to feature creation. 

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Frederick_Law]

Don't worry, no Solidworks user know it.

Not even a college Solidworks teacher.

The problem can be fix at both end:  SW export with point merge and Cutting Software (ProNest) import with point merge.

[Cadmanto]

That's great for SW, but I need to know as I asked in my earlier posting, this point merging accuracy in Inventor.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Frederick_Law]

As I said, Inventor have all end points connected.  No merging required.

Attach the RENAME DXF.

NM I see it on Kelly's post.

[johnsonshiue · Accepted solution]

Hi Scott,

I am sorry I don't know why I missed this thread. I think I know where the problem is. This is actually a bug/limitation in the way Inventor exports two-point spline. It is not properly exported. Attached is an .ini file to force the spline to be replaced with polyline before exporting. You may need to edit the .ini file and change the logical paths. Just select the .ini file when you export it to DXF. It should work better. Please let me know if it works for you.

Many thanks!

[kelly.young]

Hello @Cadmanto let us know if the .ini file @johnsonshiue supplied works. 

It seems that the 0 Layer export worked? You might try this and see if the results come out better.

• Create an .idw drawing.
• Access Manage > Styles Editor.
• Create a  New Layer named 0.
• Delete the Border and Block so that it is just a blank sheet.
• Save As > Save Copy As Template.
• Create a new Base View.
• Window select all geometry and change to layer 0.
• When you Save As > Save Copy As > Save as type > (*.dxf) it will set it to the zero layer.
• You might have to change to Options > File Version > AutoCAD R 12/LT 2 DXF. 
• Tested by opening up in AutoCAD and it shows as 0 (instead of VISIBLE_ANSI).

If it liked the zero layer this might be the easiest way to get Inventor to create the .dxf on that layer to be read by the burn table. 

Please select the Accept Solution button if a post solves your issue or answers your question.

[Cadmanto]

Hi Johnson,

Don't sweat it.  I downloaded your .ini file and tweaked the pathing.  What I am a little confused on is how to apply/use it in Inventor before exporting out to dxf.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018