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inconsistent part geometry after 'save as' operation

6 REPLIES 6
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Message 1 of 7
designingberlin
357 Views, 6 Replies

inconsistent part geometry after 'save as' operation

I just stumbled across an issue I never had before. I wanted to save a part from an assembly file (to do some CAM on the part).

I used the 'save as' menu on the part, but the saved file has a different geometry. I tried 'export...' to *f3d but same result. Exporting to iges and reimporting to fusion worked, but still ...

 

screencast shows what happened.

 

Screencast will be displayed here after you click Post.

13a8a644-e3b0-4543-ab10-b83f4f5a6be8

 

Did anyone cam across this issue? What to do?

It makes me nervous, because if the difference is not obvious, I might end up machining wrong parts ...

 

Thanks,

Stefan

6 REPLIES 6
Message 2 of 7

You forgot to add a link to the Screencast.  Also, if you can supply a file that exhibits the problem, that would be very helpful.

---------------------------------------------------------------
Brian Ekins
Inventor and Fusion 360 API Expert
Website/Blog: https://EkinsSolutions.com
Message 3 of 7

 

 

You are right .

Message 4 of 7

What you're seeing is expected behavior.  I was worried that the geometry itself was somehow different in the exported model.  However, the difference you're seeing is that the entire part is in a different location than in the design it was exported from.  The reason for this is that you are exporting an occurrence (an instance of a component).  Occurrences can be repositioned within an assembly and you can even have multiple occurrences that reference the same component.  When you export a body that you select in an occurrence, the body that's exported is the body that exists in the component (which you don't actually see) and it uses the coordinate system of that component. 

 

There's a description of this in this section of the API help.  Hopefully, that will help.  

http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-88A4DB43-CFDD-4CFF-B124-7EE67915A07A

 

The only time when you can always expect the exported body to be in the same position as the original body is when the body exists in the root component of the assembly.  It's then exported relative to the assembly coordinate system because that is the same as the root component's coordinate system.

 

If you need the exported body to be in the same position as it was in the assembly, you can work around the behavior by copying the body from the occurrence into the root component.  This is fairly easily done by having the root component (main assembly) active, select the body you want to export.  To make sure you're selecting a body and not a component it's best to select it in the browser.  Right-click and pick "Copy".  Right-click in an open area of the graphics window and click "Paste".  Click "OK" on the "MOVE/COPY" dialog to leave the copy in the default location.  Now, export that copied body, which will be in the Bodies folder of the top assembly.  You can undo to get back to the original state.

 

---------------------------------------------------------------
Brian Ekins
Inventor and Fusion 360 API Expert
Website/Blog: https://EkinsSolutions.com
Message 5 of 7

hi Brian,
please note that I'm not worried about the positioning of the part itself.
The tapered pocket feature moved it's position within the body. That's
my concern.

Thanks,
Stefan

Message 6 of 7

I see it now and am able to reproduce it.  It would be best to report this on the support forum (https://forums.autodesk.com/t5/fusion-360-support/bd-p/962).  What's happening is that when doing the "Save Copy As" of a component, the contents of that component (sketches, features, construction geometry, etc.) are being copied.  When you open that part it's essentially being rebuilt from that information.  The sketch that defines the pocket must be based on a face or construction plane that's in another component and is being positioned incorrectly in this copied design.  I'm certain this problem is restricted to the "Save Copy As" and saving the component or body as STL, or STEP will be OK because they're both saving the body as it exists in the assembly.  It's still a problem though and should be reported.

---------------------------------------------------------------
Brian Ekins
Inventor and Fusion 360 API Expert
Website/Blog: https://EkinsSolutions.com
Message 7 of 7

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