DWG Issues With ACAD LT 13

[cglusky]

I need usable DWG files in ACAD LT in order to manipulate/export for custom 2D CAM processing.

If you export a DWG from Fusion and then open in ACAD LT 13 everything is in paper space.  That's OK, I'll just select the objects and move them to model space.  Wrong.  Does not work.  No active model space says ACAD LT 13.  No problem, I'll just activate.  wrong.  Does not work either.

So why can't I use a DWG file from one Autodesk product in another?

I really hope I can at least pass some type of Fusion export file through Inventor to get a usable drawing or I will have many man hours of work that is trapped in an unusable system.

[cglusky]

Seems Inventor 13 has issues with the Fusion DWG as well.  It will open and you can see the drawing, but does not seem to recognize anything but the sheet and title block as objects.  Can't select drawing objects etc.  And when you export the DWG from Inventor as DWG 2010 and then open ACAD LT 13 all you get is the sheet in paper space with a blank model. 

You can reproduce by just drawing a simple cube in Fusion 360; export to DWG; try to use in ACAD LT 13 or Inventor 13.  Why do I get the feeling that the "solution" will be to upgrade to 14.  Not an option.

Anyway, I can at least export a STEP from Fusion; import to Inventor; create a new drawing; and export to DWG for use in ACAD LT 13.

[cmiller66]

Hi cglusky,

Just so I'm sure we're talking about the same thing, can you provide a little more detail on exactly what you're doing, and the workflow you are attempting?

When you say "Export to DWG" are you exporting the Fusion design itself or a Fusion Drawings-created drawing file?  It sounds like you've generated some 3D geometry in Fusion and you are now trying to export that to DWG format for additional editing (or 2D drawing creation?) in another product, ether Inventor or LT.

Thanks,
Chris Miller

Autodesk, Inc.

[cglusky]

Creating a new drawing of 3D geometry in Fusion; placing a view; exporting to DWG; when opening in either ACAD Lt 13 or Inventor 13 the drawing objects do not appear to be usable.  Everything is in paper space in the layout viewport.  And I can't seem to get them to move to model space.

FYI, when you create a drawing in Inventor from 3D geometry; place views; and export that drawing to an ACAD DWG you get both appropriate model and paper space objects.

[cmiller66]

Hi cglusky,

Thanks for the information.  You are correct, when the Fusion Drawings-exported DWG is opened in AutoCAD LT, model space will be empty.  We do not support exporting of the drawing and having the resulting DWG contain the paperspace entities (views, dimensions, titleblock) in the Layout of the DWG and a 3D solid version of the Fusion geometry in model space.

If the goal is getting the 2D geometry contained in a Fusion Drawing into an editable format in model space you can do the following:

1.  With the drawing active in Fusion > Output DWG from the toolbar (Note: This is a one-way trip that breaks associativity with the Fusion design)

2.  Open that exported DWG in AutoCAD LT > Layout should be active and show the views, dimensions, titleblock

3.  Use the EXPORTLAYOUT command, this will export all of the contents in paperspace to modelspace in a new drawing

4.  Open that drawing > View geometry is now a block > Explode it and you have your 2D geometry.

The intent is that the Fusion 360 Drawings feature will ultimately be the detailing/documenting tool for Fusion designs so exporting for use in another application will not be required.  If there are tools you need that are not yet there, please let us know - this will help us prioritize future feature work.

Thanks,
Chris

[cglusky]

Chris,

Thanks for the info "exportlayout" is a new command for me to memorize.  I had already processed all the models through Inventor to get what I needed, so iw ill try that next time.

BTW, I am NOT looking for "a 3D solid version of the Fusion geometry in model space." from the DWG.  Obviously, when you place the views of the 3D geometry in a Fusion (or an Inventor) drawing it becomes a 2D representation of one or more sides of the object.  I think most people would expect them to be 2D.  Just like in the layout.  The problem is you have to go through extra steps, as you have indicated, to place the 2D drawing objects into model space so you can do anything useful with them for 2D CAM or other post operations.  Perhaps an edge case, but still frustrating when I can export a DWG from an Inventor drawing and not have the same issue.  I guess I was expecting a bit of consistency across products and file types.

R,

C

[Anonymous]

Hi Chris

im using Bricscad v13 and having the same issue

- if i export a drawing to DWG the line work is in paperspace and is non-selectable

- dims and sheet are ok and can be selected

is this a bug??

Andrew

[cmiller66]

Hi Andrew,

The drawing created in Fusion 360 drawings references the Fusion design, so you're right, the exported drawing will be a layout containing title block, views and annotations and there will be nothing in model space.  That is expected.

I'm not familiar with Bricscad, but it's likely that the AutoCAD Drawing View object we're using, which is a relatively newer object in AutoCAD, is not as fully supported as objects like dimensions which have been around for a long time.

Currently you can export a sketch from the Fusion 360 design to DXF by right-clicking the sketch in the browser and selecting Save as DXF. We have plans to add Output to DXF for drawings (this would also need to export the layout to model space and explode the drawing view objects) but I'm not sure when,  The Fusion 360 Roadmap hasn't been updated yet, but you can check back there for details on what features are coming next.

Thanks,

Chris