How can I unbend square to ellipse blend in creo sheetmetal? I am using sketched rip.

[sbhattacharya-2]

Dear Creo users ,

I am using creo software for three years. I am stuck with a problem. I can unbend square to round creo blend sheetmetal but cannot unbend square to ellipse blend shhetmetal. i am currently using creo 2.0 but managed to use creo 3.0 also.In both softwares I am having problems unbending it. in PTC Creo learning exchange or You Tube  I could not find any tutorials regarding this.

My previous post was a mistake as I use full caps in my post. Other Creo users in community has pointed out .That was a mistake. I am so sorry and apologize for that. I am new in this community did not know the rules but now I know.

I need help regarding this problem. I have attached two creo 2.0 prt files. Anyone is free to answer this question. Other creo users in my company are also facing this problem in square to ellipse blend unbend problems. If this succeed it will be immense help for me.

With regards,

Soumya Bhattacharya

[StephenW]

Creo sheet metal will not work with the part as designed. Creo sheet metal requires constant radius bends. Your bends transition from a 20mm radius at the bottom to an ellipse at the top.

There are tools in surfacing to flatten surfaces but that is not something I use.

[sbhattacharya-2]

Can I unbend any blended sheetmetal part with different profiles? Constant radius bend I think is not possible in complicated hopper type part which is circle or ellipse in one side and other is rectangle.

[StephenW]

There is a significant discussion here Flat pattern of a part which was created using a Swept Blend about flat patterns for parts similar. Maybe it will help

[StephenW]

And another similar one Part to unbend

Both of these examples using multiple bends to achieve the desired shape, which, in my experience is very common practice in certain manufacturing environments. Your only other option would be custom tooling to fabricate the part, which tends to be expensive, but may be practical in large quantity manufacturing.

[sbhattacharya-2]

I am using Creo since three years. Sometimes I use Solid works. I think this kind of unbending of complex blended sheetmetal hopper like parts is not directly possible by direct unbend option in creo sheetmetal. I think I should use flatten quilt or flatten quilt deformation option in creo part modelling. But if the same part u try to unbend in solid works or solid edge it will easily unbend with just the unbend tool. This unbend option is creo do not works with complex blend profile. I think this only is a serious drawback of the software creo. This problem is not solved in creo 3.0. May be I hope this unbend option in creo sheetmetal for blend and swept blend profile need to be updated in coming version. The software Creo is very useful software and is ahead of other cad/cam software with its useful options. But this is seriously a drawback. Creo sheetmetal unbend option needs to be updated.

[StephenW]

You say that solid works and solid edge does the unbend but does it understand the math behind the unbend. It solidwork/solidedge actually calculating the bend allowances and giving you accurate results that are manufacturable OR is it just actually doing the same thing that the flatten quilt option does in Creo, only calling it a sheetmetal unbend operation that is giving misleading information. I have not used solidworks for sheetemetal operations so I don't know the answer, but I caution anyone that is using the software to verify that the information it is presenting is correct.

I would also caution users of CREO that the sheetmetal flat pattern is giving information based on a k or y constant, which is specified in the model properties and that if you are using an incorrect value for the K or Y constant, your flat pattern is incorrect.

It is very important to understand what the software is doing, no matter what software you are using.

[sbhattacharya-2]

Yes Stephen after your post I have checked Solid Works and solid edge but in Solid Works I also see the K and Y factor option.  But I also think Creo is more practical and more related to mechanical engineering but making or creating complex hopper like part which relates to blend option in Creo sheetmetal and unbend it, I should be thinking twice before doing it in Creo rather it would be easy to create in Solid Works as it unbends fast. What do you think?

[dschenken]

I think I would like to see the machine you are using that makes the variable radius bend.

[sbhattacharya-2]

Hi creo users,

I request other creo users to create ant try to unbend a square to ellipse blend in creo sheetmetal. If you get any solution please reply in this post. with creo planar, extrude, flat and flange option a part sheetmetal can be unbendable but when you use sweep or blend the sheetmetal part is unbendable.What do you think?

With regards,

Soumya Bhattacharya

[StephenW]

The links are how users do it for Creo and that are manufacturable without custom tooling.

Flat pattern of a part which was created using a Swept Blend

Part to unbend

[psobejko · Accepted solution]

As others pointed out, blended sections can be developed into a flat pattern provided that the formed surfaces are not twisted.

The example ellipse to square transition, (or rather rounded square) is presented here:

Examine the attached model (Creo 2.0).  By manually constraining the sketch entities, I ensured that edges in the rectangle 1/4-section are parallel to corresponding edges in the ellipse 1/4-section section.  There are a lot of variables as to what spacing between the vertices should be and this can be optimized but Creo just does not have an automated way of blending sections by "developing" / "triangulation" techniques (Solidworks does).  The method presented is by no means "easy to use", and the resulting model is rather rigid and brittle.

[sbhattacharya-2]

Hi Paul Sobejko, I think your method is the most appropriate and correct way of doing this.Thank you very much for your kind reply and effort.I thank you personally. I have a question.Should I have to divide the ellipse and rectangle's 1/4th section in 10 segments always? because you see I have attached a model created by your process but I have not divided it in 10 segments I have divided it in 3 segments and use sketched rip but it doesn't open or unbend. What do you think? I have attached it here.

With regards,

Soumya

[psobejko]

You missed the key aspect of the process: approximations of your curved sections using straight line segments!

And then imposing the parallel constraints on the corresponding straight edges of the two sections...

[sbhattacharya-2]

Hi Paul, I have tried again by the method. I really missed that point. But now I have been able to unbend half. Why is it not fully unbend? I have attached the model.

With regards,

Soumya

[psobejko]

The problem is in Sketch 3 - two of the segments have the parallel constraint on them.  The rest don't and so you don't get the fully flat un-bend...

Try to make every set of edges parallel, like this:

This can be tricky.  One thing that helps is to remove the coincident constraints at the two ends of the round in the square section.  Good luck!