Bug: 2D Drawing exports with 3D bits in it (Simplified DWG)

[alan.jonesXHXUF]

Exporting Simplified DWG is a feature I've been craving for ages ... and now it's here it's not helped me much because it seems to export 3D geometry rather than a 2D drawing! 

Here's what I see on my top plane... a nice 2D drawing 2019-09-26 16_39_05-Greenshot.png

But when I tried to edit stuff...well it all went weird because it's not 2D curves, it's 3D geometry! Here's the side view, showing the random portions of my model floating round above the rest of the drawing, which is the horizontal line. 

2019-09-26 16_39_26-Greenshot.png

[sabadell]

Hi,

Can you be more specific, when you say "it all went weird"? We are aware that the geometry is not fully flattened in the Simplified drawing, but as you point out, it looks correct in the top/plan view, and should also plot correctly.

Thanks.

[alan.jonesXHXUF]

Weird as in can't select anything properly for dimensioning etc or modifying the drawing as 3D stuff has different workplanes and co ordinate sytems etc...that kind of weirdness.

In short it's no more useful than the base drawing in Fusion, which is pretty useless, hence opening it in another 2D Cad program to further edit  the drawing in the first place.

[g-andresen]

Hi,

if you made the export via File > Export you will get a 3 D-file.
For a 2 D file you have to export the view e.g. as DWG or recently also as dxf via the drawing mode.

günther

[alan.jonesXHXUF]

No you don't, you get a weird hybrid mix of 2D with the odd bit of 3D, as illustrated in the screenshot above, which is neither use nor ornament. If it was a full 3D model, you could do something with it - but why would you want to export your 2D drawing as a 3D model? You wouldn't, you'd open the 3D model file! 

If you export 2D, you should get 2D. 

[HughesTooling]

This is expected behaviour but not too helpful. In whatever program you're going to export to you'll need to flatten the design. Below I made a screencast for someone else to demonstrate the problem, in ZW3d scaling the Z by zero works or Rhino ProjectToCPlane works. Seems we'll need to request a flattened drawing on the ideastation.

Mark

[sabadell]

Hi all,

Thanks for adding some detail to this concern. When designing this feature, we were not concerned with "flattening to 2D", and perhaps this reflects a lack of understanding of the specific workflows you want to use this export format for.

Just to be clear about what we are talking about:

• An Export to the "AutoCAD DWG" format preserves all your sheets in a multi-sheet drawing. However, it requires that destination application be an Autodesk product due to the complexity of the "model documentation views". This format preserves all of the intelligence and complexity of the source drawing except that you can no longer update the views to match changes to the model.
• In the September release we added a "Simplified DWG" format, and a separate command to export to DXF. Both of these are the same, except for the files being DWG vs DXF. This format takes a single sheet and "explodes" it; it simplifies things to more basic geometry. This has the advantage that you can open this drawing in non-Autodesk CAD applications (as long as they support the AutoCAD 2013 DWG format). You lose quite a bit through this process, however. Most significantly you just get one sheet per drawing. Second, if views are scaled (and not 1:1) in the source drawing then the simplified geometry in these exported files are scaled. This means that adding dimensions to this drawing may require setting a linear scale factor on the new dimensions.

In order for us to make "flattening to 2D" a priority it would be super helpful if you could explain the specifics of your workflow: why are are exporting to this format, what tool you are using (or want to use), and why you feel it should be strictly 2D - what problems it causes given that it contains some geometry with coordinates where Z != 0. I am particularly interested in the mention of editing view geometry - what sorts of changes are currently not possible in Fusion, that you are making?

Sorry this feature did not meet your expectations; helping us understand these workflows will really help.

[HughesTooling]

For me the use would be subcontracting flame\plasma cutting. You need a 2d drawing with dimensions and specs so exporting a sketch is no good on its own. In the past with other solid modeling programs I just create 2d drawing from the part and export. With fusion in the past you'd need to export a sketch and create a 2d drawing and export as a pdf. The hope with the simplified export was a 2d drawing with dimensions. The flame cutters can import the DXF and they have dimensions to double check against for scale.

I've received DWG and DXF drawings from customers using Inventor and they have always been 2d so was a bit surprised by the Fusion export.

Thanks Mark

[m.podsiadlowicz]

Hello.
I have the same problems with "flat" fusion drawings and their export to DWG.
These drawings are not flat. Why do you keep the "Z" dimension on the flat documentation.
It is obvious that it should be reduced to 2 dimensions.
I have written about it in many of my submissions.

[m.podsiadlowicz]

Hello.
I have the same problems with "flat" fusion drawings and their export to DWG.
These drawings are not flat. Why do you keep the "Z" dimension on the flat documentation ?
It is obvious that it should be reduced to 2 dimensions.
I have written about it in many of my submissions.

[sabadell]

Hi m.podsiadlowicz,

This information, from an earlier reply, would be really useful, for your specific workflows:

"In order for us to make "flattening to 2D" a priority it would be super helpful if you could explain the specifics of your workflow: why are are exporting to this format, what tool you are using (or want to use), and why you feel it should be strictly 2D - what problems it causes given that it contains some geometry with coordinates where Z != 0. "

The problems I see with re-purposing an annotated drawing to use in workflows that are bothered by geometry that is not completely flat:

• Drawing views might not be 1:1 scale
• Views might have hidden lines displayed (they can be turned off)
• Geometry limited by sheet size
• Sheet often contains title block and border (though they can be turned off), as well as text and dimensions
• Drawing might be multi-sheet

These seem, to me, to suggest that a more direct solution would be far better; a feature more like "Export 2D geometry to DXF" that would avoid sheets and scales entirely.

[m.podsiadlowicz]

HI.

Then maybe I will ask a simple question:
What is the purpose of keeping the information about the depth of space in the drawing of the flat technical documentation, i.e. the "Z" dimension ?

What is it useful for when we project an image onto a "flat piece of paper"? 

After all, if we need to export to 3D .DWG, we do it from the level of the 3D model.

For what purpose was this function prepared?

Who needs the "Z" dimension in flat drawing export? 

Maybe the program team has hit a dead end and cannot fix it?

[sabadell]

Hi,

While I did not write the code that "does the math" to generate the view geometry (hidden lines removed or shown dashed, profile edges in heavier line weight, calculations for interference edges, etc.), I suspect it was simply a matter that it is easier (in terms of code) and faster (in terms of computation time). Flattening 3D geometry, when you have curves seen obliquely, is a more complicated operation. In addition, say you do see a curve obliquely or on edge, but you want to dimension the radius or diameter. If you flattten the curve, and it is then represented in a tessellated form, it becomes more difficult for the dimensioning tool to "see" that it is actually a curve, and provide an accurate radius or diameter. It would instead see a bunch of short straight line segments.

Understanding your specific use case will help us ensure that in the future we either change our view generation, or provide an alternative path, that will meet your needs. Thanks for the feedback.

[m.podsiadlowicz]

Hello.
I understand the need for the visibility of inclined holes and curves and problems with presenting them in the "XY" plane.
Sure, they're not the same curves anymore.
However, there were no problems with projecting onto a plane in the 3d sketch area (solid) and the math apparatus is there for that.

As for the dimensioning of projections in the technical drawing.
Usually, we do not dimension curves and holes in ambiguous positions of the planes.
For dimensioning, the detail should be set in the drawing so that it is seen correctly parallel or perpendicular to the plane of the paper sheet.
It is impossible to show the dimensions of an arc correctly if it is shown at an angle other than "n x 90deg".
The "drawing" module should go from the idea of an old-fashioned drawing board and ISO standards to flat documentation.
Everything else leads to a CAD builder misunderstanding by a mechanic, turner, or CNC operator.

This is not "coreldraw" 🙂
regards

[m.podsiadlowicz]

I work with workshops that have very old Autocad versions and old machines.
They don't own Fusion360 and they won't buy it for sure.
They have to get "flat" DWG drawings from me ("XY <> 0; Z = 0), where lines do not coincide, do not duplicate and are connected end to end.