Unroll curved surface/cylinder

[Anonymous]

Is there a way to unroll and create a 2d profile of the circumference of a cylinder or curved surface in inventor? I know solidworks has a flatten feature and the reason I ask is it's extremely useful for printing out a 2d pattern for notching tube ends such as for car chassis or framework. You can roll the paper pattern around the tube end and simply cut along the line. I prefer using inventor and already have the software and I'm not crazy on trying to download an add-on but if I have to so be it.

[johnsonshiue]

Hi! In a sheet metal part, if the roll is created by Contour Roll feature, you can use Unfold command to unroll the rolled part. After that, you can use Refold feature to roll it back. Please try it and see if it works for your case. If it does not, please attach the file here.

Many thanks!

[JDMather]

I use exactly the same technique in Inventor that I use in Solidworks. 

Do you have an example file that you can attach?

What version of Inventor are you using?

[Anonymous]

The part is an ipt. I'm using Inventor Pro 2017. It is a tube for aircraft landing gear. I want to unroll the 360 degree circumference of the tube ends to a 2d surface so I can wrap It around the actual tube and cut out the line to make a notched tube. I know solid works has a dedicated feature for this exact reason. I've attached one of the tube ipt.s please excuse the mess of planes and axis if I forgot to turn the visibility off.

[JDMather]

First thing I noticed is that you have unconstrained circles for you tube profiles - this is a dangerous practice in Inventor or in SolidWorks.

I Derived Component your tube as a surface body into a new part file.

Any changes you make to your original would be (if I didn't Suppress the link) associatively updated in the derived component.

I set the Sheet Metal thickness to be equal to the thickness of a sheet of paper (.004in).

Thickened the outside surface.

Ripped the result.

Flat Pattern.

See attached file.

[Anonymous]

Thanks for that. I'm always happy to learn so what is the proper way to do tubing models. They are kind of they're own type if model in a way. Did you say you did it in sheet metal? I haven't had a lot of experience with sheet metal but should take a look into it and do some practice.

[JDMather]

I would use Frame Generator to create the frame.

I would then Derive Component each frame member into sheet metal part to get the flat pattern template to wrap around actual tube for hand cutting.

[Anonymous]

I've done some work with the frame generator. Excellent feature but as far as I can see it has every imaginable type of material except what you'd expect it to have. I'll be building out of 4130 tubing 1.25"×.049" but standard tubing in inch sizes is nowhere to be found in the content center.

[Anonymous]

You can add your own customs profiles. see https://www.youtube.com/watch?v=XOwR89pA_e8