Converting Part to sheet metal flat

[Anonymous]

Part of my job is to lay out blanks of 3D models so the blank can be sent out and cut.  Is there a way to convert an Inventor ipt file to a flat blank?  I have tried "convert to Sheet Metal" but Inventor reads the pre-bent part as the flat layout.  I am currently using Inventor 2013. i attached a drawing for an example if anyone can show me how.   

[JDMather]

For any chance of this part returning a flat pattern you will have to use the Sheet Metal tools to model.  Even then, not sure it will return correct flat pattern.

[Anonymous]

Im not sure what you mean by sheet metal tools. Are you saying recreate this part in the sheet metal format?

[blair]

This part would be produced using a stamping method with a set of male and female dies. You created this item just using the Part template and not the Sheet-Metal template, a different set of tools.

Start with the Sheet-Metal template, create your flat bottom and then the flanges, you might be able to use the rolled contour tool to develop the offsets. Or sketch a line to the outside profile and extrude to surface, then use the Thicken tool to get the proper thickness, then use the Contour to develop the offsets.  I really think that this is outside of the S-M module in Inventor.

You might look at a 3rd-party tool such as AutoPol

[Anonymous]

So basically you are saying a fully bent model made in ipt format cannot be laid out as a flat sheet metal without recreating it in the sheet metal template? I get most models sent to me (in ipt) so recreating them would not be time efficient.  But thanks, i will look into the software you listed below.  At least i dont need to waste time trying to accomplish this anymore!

[JDMather]

Generally here is no difference in creating with sheet metal tools or the standard tools as long as the part is one that can be folded on a press brake.

The problem with this particular part is it is a draw formed die part - not a folded part.

In some cases Inventor has gotten around that with Contoured Roll and some Lofted Flange features, but I am skeptical about this particular part.

If there were some Rips in these areas then the part could be made on a press brake.

[Anonymous]

I get what you are saying.  I guess my main question is; Is there an easy way to take an ipt model and get a flat layout of it?  Completely recreating the part in the sheet metal format is not going to help me.  I need to take a pre-made part and lay that out as a blank to save time.  Is that possible?  I am assuming not.  I attached a different model without the offsets.  

[blair · Accepted solution]

Convert to Sheet-Metal, go to Sheet-Metal Setup, set your thickness to the 3.42mm and the model will flatten. As is done in your sample.

[blair]

The only thing that you may need to change is the k-factor. Each machine and bending process most of the time requires a different k-factor to allow to develope the correct flat layout.

[Anonymous]

You answered both parts of my question.  Originally i tried adjusting to the correct material thickness and it didnt help.  Now i realize its because i chose a part that would be produced using a stamping method.  I just assumed i was doing something else incorrect.  I can at least use this for 50% of my blank layouts.  Thanks!

[Anonymous]

Hi,

I made this as a part using sweep option. I need to flatten this part. I tried to increase the thickness. But I am not able to use the rip option. Is there any option to flatten this part?

[JDMather]

You did way to much work to create a simple part - all you needed was one sketch with one circle and to a Rotate instead of Sweep.

In any case, Inventor will not produce a correct flat pattern for that part.

You could use the Contour Roll to create the part, but the flat will not be correct.

[Anonymous]

Thank you. I tried with contour roll. The flat pattern obtained for the bend is a rectangle. Is there any method for a better flat pattern?

And one more doubt how to dimension the flat pattern?

[JDMather]

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@Anonymous wrote:

... Is there any method for a better flat pattern?

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Other software (or add-in) or manual layout in AutoCAD.

[Anonymous]

I've attached a simplified version of a gored elbow. It contains 4 files: a Reference part, an End Gore part, a Mid Gore part, and the Assembly file. This is typically how you would make an elbow out of sheet metal for use in duct work. It's easy to form and assemble, plus it gets the job done. Generally, the seams are staggered (alternating sides) for strength. I'm sure you could make the assembly do this for you (alterante sides for seams), but I think it would require some iLogic code.

[RasmusBredal]

Hey All

It is possible to make a Elbow and unfold it, in one Sheet Metal.

Taking Sheet Metal to the next level.

[JDMather]

You changed the problem.

That is not the problem as described in this thread.

I would not use your solution even for the problem as you have changed it as it is not an efficient use of material.

I have posted the correct solution to the problem of elbow gores as you have changed the problem many times in the past.

[Anonymous]

Hello,

I converted step file in ipt , but I can't convert the ipt model in sheet metal. I followed the procedure about set the thickness, but Inventor don't do it,  dont make flat pattern, I don't know what is the problem....Somebody can help me , please?.... I Got this step file from a customer... it seem that he set the inside bend radius =0, and bend radius outside was set equal to thickness, I don't know if the problem is because of this....

[Anonymous]

I am working with Inventor 2011

[JDMather]

Zero radius bends were not introduced until r2015 (or maybe it was the current release 2016).

A bit of cheating should get it done in 2011.

Delete Face all of the inside and connecting faces.

Set your sheet metal Thickness to .059 (instead of .060)

and then Thicken your part towards the inside by Thickness.