AutoCAD to Fusions - pline - spline issues

[Pshupe]

I have a bunch of guitar designs in AutoCAD and I would like to use them as backgrounds to develop fusion models.  When I insert the dwg files some of the lines come in fine, while others do not.  Namely splines and plines. Also the Fusion file is very unstable.  I assume it is the number of segments in the splines or plines?  What is the best way to  bring these files into Fusion so I can use them as a background and sketch using "project" to select faces to extrude?  Thanks.  Regards Peter.

[jeff_strater]

Hi @Pshupe,

If you are just looking to use these as a visual reference, you can place an image of the design as an Attached Canvas, calibrate it to the correct size, and sketch the design following the curves.

However, you should be able to just insert the DWG/DXF into Fusion.  If this is not working correctly, can you share the ACAD design file with us, so we can track down the problem?

Another approach, if you think there are too many line segments, is to simplify the ACAD drawing by separating into multiple designs.  One for the body outline, one for the pickup pockets, etc.

Jeff

[Pshupe]

Thanks Jeff - I'd like to use this to push/pull a Fusion component.  I've tried a number of times even starting with geometry that I draw with plines and splines in a fresh AutoCAD file.  It just does not seem to like curved lines from dwg.  Obviously this is a huge issue as I can easily redraw straight lines but redrawing a curve is more time consuming and doesn't seem to result in as smooth a final product depending on how many splines I use in Fusion.

I have attached a spline created in AutoCAD, saved out as v 2013.  Drawn as a pline that is smoothed into a spline.  When I insert into a design or just drag and drop into a saved fusion file, it does not appear. Here is how it looks inside AutoCAD. 

It doesn't get much simpler than this.  I do not mind splitting up an AutoCAD file into pieces if that helps, but this doesn't even show up in Fusion?  Thanks for any help.

Regards Peter.

Thanks Jeff - I'd like to use this to push/pull a Fusion component.  I've tried a number of times even starting with geometry that I draw with plines and splines in a fresh AutoCAD file.  It just does not seem to like curved lines from dwg.  Obviously this is a huge issue as I can easily redraw straight lines but redrawing a curve is more time consuming and doesn't seem to result in as smooth a final product depending on how many splines I use in Fusion.

[jeff_strater]

thanks for the file, @Pshupe,

I was unable to import this into either Fusion or Inventor as a part.  I'll have the team look at this to see what the problem is.  Can you export this as a DXF, and then try inserting it into a sketch?  Just something else to try.

Jeff

[Pshupe]

I exported to dxf and it seems to upload better.  The outline at least shows up in the preview.  When I load it into a project though it shows up then disappears, and freezes and crashes.  Is Fusion made by Autodesk?  LOL  It sure doesn't seem to like anything AutoCAD???  It's pretty frustrating.  It's bad enough trying to learn a completely new / different software.  I'm not sure this is useable for my workflow.  Oh well.  Thanks.

Regards Peter.

[Beyondforce]

Hi @Pshupe,

Until @jeff_strater 's team will figure out the problem with the DGW file, you can use THIS technique to import your drawings into Fusion. I have used a Foxit pdf to open the DWG file and to convert it into an image file, but you can also use adobe pdf as well.

I have attach the a result file. If you have questions, please let me know.

Cheers / Ben
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[Pshupe]

It would be nice to keep this as a vector.  I assume you lose the size of the geometry by doing this?  It's hard to believe it is so difficult to bring something from Autodesk AutoCAD to Autodesk Fusion?  Is this not done in Inventor all the time?  Thanks I'm looking at other options for export and import into Fusion.

Cheers Peter.

[Beyondforce]

@Anonymous,

This is a quick workaround until the Fusion team will figure out the problem. Yes, the size of geometry is lost, but you can restore the size with just a bit patience.

Sorry I cannot be of more help!

Ben.

[HughesTooling]

I've found the settings here work for Rhino, don't know if AutoCAD has equivalents. Attached DXF exported from Rhino.

Mark

[eellenburg]

It appears that the Fit/Smooth type of the polyline is what Fusion chokes on.  It imports fine if you use "Curve Fit" instead of "Cubic" or "Quadratic".  Only problem is this changes the outline slightly.

Another way to import your shape is to extrude the profile into a solid in AutoCAD & export as a SAT file.  You can then upload the SAT to Fusion.

[jeff_strater]

@eellenburg has hit the nail on the head.   Apparently, it is that type of spline in particular that is the problem.  For reasons that I don't understand, Fusion does not recognize that kind of spline entity.  We are looking into why that is the case.  But, in the meantime, some of the other suggestions here would be a good way to go.  Change the curve type in AutoCAD, create a solid in AutoCAD, or just import the image and re-trace the curves in Fusion.

Jeff

[Pshupe]

How would I change a "Fit / Smooth" polyline to "Curve / Fit"?  Is this a setting in AutoCAD or in Fusion?  Thanks.

Regards Peter.

[eellenburg]

AutoCAD.  You can see a screenshot of it in my previous post above.

Open the properties dialog (Ctrl + 1).  Click on the polyline.  Find "Fit/Smooth" under "Misc" in the properties dialog.  Change from "Cubic" to "Curve fit".

[Pshupe]

Thanks for the tip.  That seems to work better for getting the spline to actually show up, but when I create a component, new sketch, push-pull the outline it shows every point in the spline when I extrude.  Funny thing as well, if I trace over it with a native spline inside of Fusion 360 it also gives me the same thing.  It also seems to be very heavy graphically.  The program gets minimized for a while until it calculates the solid and then it comes back.  I find this hard to believe that this is the best workflow for creating a basic outline that is not straight lines??  Or is Fusion just not good with curves?  Thanks for any advice.

Here is a screenshot of the imported spline extruded, which looks identical to one that I draw inside Fusion using the outline as a guide for tracing on top with splines.

Regards Peter.

[Pshupe]

So even re-tracing the curves in Fusion results in this faceted solid?  I just used the spline command and traced over the outline.  I did place a lot of points, which is evident by the number of facets.  Would it be better with less points?  I'll have to test.  I've drawn this outline and imported different files about 20x now and I don't feel like I'm any closer to getting a nice solid at the end.  One thing good is that I only have to create this once and then use it for CAM toolpaths.  It's always frustrating to learn a new software and I really hope there is a better way to create a nice un-faceted curve so I can develop more of these models as I need.  Thanks for all the help.

Regards Peter.

[HughesTooling]

I think the problem you have is while tracing every click is creating a copy of the underlying curve. See screencast. One workaround might be to hold the Ctrl key down while tracing to disable snaps.

I'll add the screencast when I can. at the moment the site will not let me view or manage any of my screencasts.

Mark

[Pshupe]

Thanks Mark - I'll give that a try and see if that helps.  Looking forward to the screencast! 😉

Cheers Peter.

[HughesTooling]

Here's a screencast that shows all the copies created while tracing. I think this might be a new problem because I've done stuff like this before without it creating all the copies. I have auto project on reference disabled so I'm not sure I should get any copies.

Here's another idea to get around the problem. Create a component and make it unselectable while tracing.

Mark

[jeff_strater]

@HughesTooling is correct if you are adding the spline in a new sketch (snapping to the curve in another sketch will auto-project the curve into the active sketch).  So, I would recommend editing the main sketch when doing the re-tracing.  Another consideration is that the faceted curves will also be recognized for the extrude.  I would recommend first converting all of those curves to construction before doing the tracing.  See the video below (which I made for a different thread, also on guitar design) for how I would approach this re-tracing problem:

Jeff

[Pshupe]

Thanks Jeff, Mark, eellenburg and others.  This seems to work OK.  So adjusting the spline so it shows up and then tracing over an unselectable component seems to work OK.  Once I trace with small number of points I add points as required to shape the spline to the correct shape.  I will create the dwg pline file that only has the outline.  The rest of the lines can be in another file that I will use as a reference to sketch the other details.  Thanks again.  I wish I could just import the spline and push/pull, but this seems a reasonable work around.

Regards Peter.