Bug: Export DXF DWG

[Anonymous]

Hi,

Noticed that exporting a drawing as a DXF or DWG results in an unreadable file or a blank file.

[HughesTooling]

How are you exporting? From the 2d drawings workspace did you specify the simplified versions of DWG\DXF? Have you got an example file you can share here?

Mark

[alan.jonesXHXUF]

I get the same if I export as DWG and open in TurboCAD 2019. if I export simplified it works. (All from 2D Drawing space)

[g-andresen]

Hi Mark,

I just tested it.
The Result:

DXF Export Fusion > ACAD & QCAD 09.26

günther

[HughesTooling]

@g-andresen  QCad does have some problems reading some of fusion's splines. I can't use QCad anymore as I've run it 100 times so now it will not even work as a viewer. Not going to buy as I have Rhino but it was useful to point other users to QCad.

Anyway here's an example of a simplified DWG export in Rhino. Comes is nice and clean, all simple lines, acrs and ellipses.

Mark

[Phil.E]

@Anonymous 

Sounds like you may have a bug. Let's be clear first.

Prior to the latest update, Fusion exported drawing sheets as .dwg for consumption in AutoCAD. They contained model views in paperspace. If you don't know what that means, no worry, but like all .dwg made this way they open in other applications showing the empty paperspace viewports.

Now there is "Simplified .dwg" and "AutoCAD .dwg" The former being new, and able to open in other applications that only read model space dwg.

Same with dxf sheet export. It should be identical to Simplified dwg. 

But you mention that dxf is creating empty files. Is this verified by trying to open them in another application? As you can see in the other posts here, not all applications correctly read dxf. 

Thanks,

[Anonymous]

Re: Exporting DXF/DWG from Drawing Sheets

Hi Phil,

Latest update installed on Windows 10.

Tried opening all three versions (Autocad DWG, Simplified DWG, and DXF) in Illustrator.  I receive the following message for each file:  "The file 'xxx' is in an unknown format and cannot be opened."

Tried opening all three versions (Autocad DWG, Simplified DWG, and DXF) in Solidworks.  The Simplified DWG and DXF open, but the vector/spline output is incomplete on both versions (see image).  The Autocad DWG opens, but there is no data present (it's a blank canvas).

[HughesTooling]

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@Anonymous wrote:

Re: Exporting DXF/DWG from Drawing Sheets

Hi Phil,

  The Autocad DWG opens, but there is no data present (it's a blank canvas).

---

The Autocad DWG can only be read by autodesk products so you're not going to be able to open that file in Solidworks, as explained in post #6. Have you got any example simplified files with problems you can share here?

Mark

[Phil.E]

@Anonymous 

Perhaps we should also discuss your intended workflow.

When you export a dwg, or dxf, what do you intend to do with the data? And what software are you sending it to for this purpose? I'm asking so I can test your workflow to ensure we're on the same page here and provide you with the best experience we can, according to your expectations.

[HughesTooling]

Just out of curiosity I made a part with a fit point and control point spline, created a drawing and exported as a DXF then opened in Rhino.

All looks good to me. The fit point spline comes in as a degree 5 spline and the control point as a 3.

Mark

[Anonymous]

Hi Phil,

Thanks for your reply.  I'll export a DXF/DWG for illustrative purposes like making manuals/instructions or for other  illustrations/artwork.  Also, will use them for cnc/laser paths.  A lot of times it's needed to set specific views and export that view.  Having these as vectors is key to working with them in Illustrator or similar programs.  None of these files even open in Illustrator.

Regardless of workflow, if these export options exist, they should just work.  When they don't open in one program it's no bueno.  When they import into another program with incomplete lines it creates more unneeded work to fix.  Maybe it's a bug?  I appreciate you looking into it.

[Phil.E]

@Anonymous  Thanks for responding.

The dwg/dxf export from Fusion drawings is 3D. You have to project the objects to a plane in your downstream software to use them for contour cutting.

The workflow for using dxf for contour cutting is: export a sketch as DXF. 

1. First make a sketch
2. Project all the geometry you want to cut into it.
3. Export the dxf by right click on the sketch.

And regarding your comment about the exports and other software. If only it were so easy for Autodesk to force all other software companies to consume dxf/dwg the same way. But we cannot. Likewise, we cannot possibly make dwg/dxf that are universally consumable in other softwares, the standard is not always perfectly used by other companies. We just cannot support all those other applications.

I'm testing the Illustrator problem you describe. What version of Illustrator are you using?

Thanks!

[Anonymous]

Hi Phil,

This topic is about exporting from the Drawing module.  While the method you describe in 3D space does seem to work without issue, it complicates deriving contours for specific views and features.  Exporting a view from a Drawing is 2D by default.

In regards to exporting for other programs, my understanding is that DXFs are a pretty universal file format for any program that can read them, so I'm not sure why any other software should matter.  It should be like exporting an STL, STEP, etc.  Maybe I'm missing something.

[HughesTooling]

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@Phil.E wrote:

@Anonymous  Thanks for responding.

The dwg/dxf export from Fusion drawings is 3D. You have to project the objects to a plane in your downstream software to use them for contour cutting.

---

Hadn't noticed that, bit of a shame. I can convert easily enough but an extra step. Don't know if Solidworks can import a 3d DXF and convert but here's how to using ZW3d. @Phil.E  I did notice a bug though, my drawing is set to mm and all defaults in Fusion are mm but the exported drawing is set to inches so it's scaled wrong in ZW3d.

This is what's set in the DXF, 1 is inches. I've attached the DXF.

Here's the screencast, in ZW3d I use a non uniform scale and set Z to zero to flatten.

Mark

[Phil.E]

@Anonymous 

The thing you are missing is that other software can consume generic file types as they see fit. 

Adobe Illustrator only supports 2000, 2004 and 2007 versions of AutoCAD DWGs. Fusion exports 2013, a 6 year old standard. At some point we might support 12, 15, or 19 year old dwg versions. Or Illustrator will endeavor to support 2013+ versions. 

And while you may expect to export drawing views for manufacturing, based on much experience doing this with other software, the drawings you get from Fusion are not for direct conversion to CNC code, instead they are for creating shop drawings. I too had this expectation based on over a decade of using Inventor drawings for laser cutting.

That said, if I was doing the Fusion workflow all those years to feed my laser it would have been just as easy. Actually easier. I used to export IDW as DWG, clean it up in AutoCAD, and then send to CNC. In Fusion I could do that all from the design. I wish I had a better answer for you. Thanks for engaging in this discussion!

@HughesTooling 

Are you sure the dxf is not unitless, and the consuming software is reading 1 to be something other than 1 mm? In Fusion and Inventor you can specify the source units. Perhaps that's an option. I'll check out the file you sent and report back. Thanks for the heads up.

[Phil.E]

Never mind. Inventor detects Inch in your file. I'll do some testing over here. Good catch!

[Anonymous]

Hi Phil,

Illustrator is able to read and import DXFs from 3D space exports (as from sketch).  Why wouldn't this be maintained for the 2D Drawings?  Seems odd to have it work in one and not the other.

Also, beyond those files not opening in Illustrator, when they open in soliworks there are missing vectors.

I understand that exporting from drawings isn't an ideal situation for some fabrication, but what about just utilizing the vectors for other artwork, etc.  If the drawings in Fusion are only meant to be for shops, why have the feature to export DXFs from drawings?

[Phil.E]

Good question about model export. It may be that sketch export is using an older dxf standard for consumption by older cnc software, and for sure drawings exports are intended for drafting applications. Those may need some of the features in the 2013 version type. I'll have to ask.

The export options for drawings are purely intended to support other drafting applications. Not CNC, not any 3D modeling applications.

There is some information in the what's new blog.

https://www.autodesk.com/products/fusion-360/blog/september-23-2019-product-update-whats-new/

Because of this, if you look "top down" on the geometry, it forms the views you expect to draft in 2D, and it works for the users that need it. If you need a 3D view of your model in SolidWorks, just export the model from Fusion as a file type that it can open, such as .step.

If you need to make sketches for export, and are worried about viewing angles, you can make Named Views that match those angles, probably with the help of construction planes and the Look At command. These named views also can be called in drawings as "auxiliary views", but we've been down that path already.

Thanks,