Inventor General Discussion

Inventor General Discussion

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anton.zhyzhyn
Posts: 2
Registered: ‎03-26-2013
Message 1 of 7 (319 Views)
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Unable to flat-pattern a part

319 Views, 6 Replies
03-26-2013 09:23 AM

Attached. Unsure as to why convert to sheet metal then 'create flat pattern' doesn't work?

 

The full part, from which the part is derived, is in the file too (suppressed).

 

(I believe all these panels should be identical so need a flat pattern profile for one of them only)

 

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mcgyvr
Posts: 6,832
Registered: ‎12-01-2004
Message 2 of 7 (316 Views)

Re: Unable to flat-pattern a part

03-26-2013 09:26 AM in reply to: anton.zhyzhyn

I can't open the part as I'm still on 2012 but did you make sure you set the proper material thickness in the sheet metal rules before attempting to flatten?

 

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Down with IDW/DWG files..... Long live 3D PMI... Hurry it up already..
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JDMather
Posts: 26,543
Registered: ‎04-20-2006
Message 3 of 7 (305 Views)

Re: Unable to flat-pattern a part

03-26-2013 09:38 AM in reply to: anton.zhyzhyn

You should use Sheet Metal tools to create simple parts like this.

In particular you will be interested in Contoured Roll.

Please mark this response as "Accept as Solution" if it answers your question.
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swhite
Posts: 531
Registered: ‎11-08-2012
Message 4 of 7 (297 Views)

Re: Unable to flat-pattern a part

03-26-2013 09:44 AM in reply to: anton.zhyzhyn

As Mcgyver noted make sure you set the sheet metal thickness and sometimes I have had to select a face before selecting flat pattern, especially if not in default orientation.  Also, just because you can sometimes create a part, does not mean it can be bent out of a single sheet without stress cuts. I cant tell if your part has just one curve and is on an angle (preview is all I get- using 2011) or has curves in two directions. If all else fails try telling inventer the sheet is slightly thicker than the actual part is. Don't ask me why, but have had that make it work before on complex parts.

Steven White
Lee C. Moore, Inc.
www.lcm-wci.com
Inventor 2011
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JDMather
Posts: 26,543
Registered: ‎04-20-2006
Message 5 of 7 (293 Views)

Re: Unable to flat-pattern a part

03-26-2013 09:46 AM in reply to: swhite

swhite wrote:

....make it work before on complex parts.


The part is a simple part modeled incorrectly.

Please mark this response as "Accept as Solution" if it answers your question.
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johnsonshiue
Posts: 2,092
Registered: ‎04-30-2008
Message 6 of 7 (258 Views)

Re: Unable to flat-pattern a part

03-26-2013 03:03 PM in reply to: anton.zhyzhyn

Hi! For this particular case, Inventor should be able to unfold the sheet metal body. However, the body thickness is inconsistent with the one set in Sheet Metal Style. The problem here is with the Sweep path, which points slightly off the profile normal direction. As a result, the actual thickness (distance between front face and back face) is 1.191144677 mm, not 1.2mm.

There are a few ways to fix this issue without remodeling the geometry totally. Option A) Create Sweep surface instead of Solid Sweep. Then create Thicken on inner or outer face with the Thickness. Option B) Create Thicken (Join) from outer face with the Thickness and create Thicken (Intersect) from the same face with the same Thickenss. Either way should result in an unfoldable body.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Principal SQA Engineer, Inventor
Mechanical Design
Autodesk, Inc.

New Member
anton.zhyzhyn
Posts: 2
Registered: ‎03-26-2013
Message 7 of 7 (221 Views)

Re: Unable to flat-pattern a part

03-27-2013 08:39 AM in reply to: johnsonshiue

Vastly appreciated,

 

Best regards,
Anton

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