Inventor 2018 Curve Sheet Flatten Pattern Not Supported Multiple Bodies Exist

[marshall]

Hi Everyone,

I'm currently design a compact bin. The rear sheet of the bin is a curve sheet which will be profiled and then rolled with inside radius 1396 mm.

I have create this part in inventor but I have trouble with flatten it. I keep getting message of "Flat patterns are not supported when multiple bodies exist"

Anyone can help me get around this?

I have attached the part file here for your reference. You can get a full compact bin if you suppress extrude 5 feature.

Cheers

Marshall

kelly.young has edited your subject line for clarity: Help - flatten curve sheet

[mcgyvr]

where is the rip in the material like there would be in the real world?

what is the kfactor of your equipment used to manufacture this so that a proper developed length can be achieved?

why didn't you model it in the sheet metal environment to start with then the flat pattern will just work?

[blair]

You need to push out the "bodies" to their individual parts, then convert the top item to a sheet metal. I suspect that the chamfer you have at the ends of the curved body will not allow the item to be flattened. I suspect that you will need to use the top surface only and create a surface that can be thickened with all the edges perpendicular to the surface. Then this can be converted to a Sheet-Metal item, set the thickness within the S-M properties and then flattened.

There should be a tutorial within the Inventor Help for the work-flow from a multi-body to sheet-metal. 

http://help.autodesk.com/view/INVNTOR/2018/ENU/?caas=caas%2Fvideo%2Fyoutube%2Flesson%2F147854-course...

[marshall]

Hi,

Thank you for your replies.

The purpose of designing with the compact bin together rather than start from scratch using sheet metal is that for future use I can just update the size of the bin and the rear sheet will be updated accordingly.

I'll try Blair's suggestion to see how it goes.

Kind regards

Marshall

[marshall]

Hi Everyone,

Blair's suggestion makes me thinking about the corners of my sheet is not properly designed.

I have checked it and found the faults at the 2 bottom corners.

Cheers 

Marshall

[JDMather]

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@Anonymous wrote:

Hi,

Thank you for your replies.

The purpose of designing with the compact bin together ....for future use I can just update the size of the bin and the rear sheet will be updated accordingly.

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That is a good strategy - except that you did not model the parts correctly for sheet metal.

I am busy the rest of this week - so it would be sometime next week till I could create example of how I would model the parts.

Ahh, I see that you found issues while I was typing.

[marshall]

Hi JDMather,

Thank you for your reply.

Yes, as you said I have realised that I have modelled it wrong. Will figure out how to do it properly.

Kind regards

Marshall

[marshall · Accepted solution]

Hi everyone,

Based on Blair's suggestion of using thicken/offset to create this part, I have found a solution for my problem.

The answer is to find the intersection surface and thicken it.

I have attached the solution if anyone interest.

Kind regards

Marshall

[kelly.young]

@marshall if you want to stick with a multi body part you can use surface and thicken then use Manage > Layout > Make Components then create a flat pattern in each part. 

See the attached example and see if that helps. 

Alternatively you can also Create > Derive to get the geometry of a part as reference. 

Use View > Windows > User Interface > iLogic to bring up the ChangeSizeHere Form to edit the shape easily based on the parameters.

Please select the Accept as Solution button if a post solves your issue or answers your question.