Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Unable to flat-pattern a part

6 REPLIES 6
SOLVED
Reply
Message 1 of 7
anton.zhyzhyn
548 Views, 6 Replies

Unable to flat-pattern a part

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)

 

Tags (1)
6 REPLIES 6
Message 2 of 7
mcgyvr
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?

 



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 3 of 7
JDMather
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.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 4 of 7
swhite
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
Intel Dual Xeon E31225 @ 3.1 GHz CPU
16 GB RAM
NVIDIA Quadro 600 GPU
Windows 7 - 64 Bit
Message 5 of 7
JDMather
in reply to: swhite


@SWhite wrote:

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


The part is a simple part modeled incorrectly.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 6 of 7

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)
Software Test Engineer
Message 7 of 7

Vastly appreciated,

 

Best regards,
Anton

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report