Doesn't chamfered cone shape unbend support yet?

[hyarth]

1. make a cone

2. sketched rip and chamfer

3. failed bend back

As a result, I want to bend the chamfered sheet metal to make a cone. Is there any other way other than this?

[MartinHanak]

Hi,

please upload your model packed in zip file.

[MartinHanak]

Hi,

bend.prt.1 was created in Educational Creo 9.0 version, therefore I cannot open it in Commercial Creo 9.0 version.

Please use pictures and text to provide more detailed description of your model. This enable me to recreate the model on my PC.

[hyarth]

- sketch1's diameter is 1100, sketch2's diameter is 916, height is 2000, then I was blended.

- then I creat DTM3 to rip

[MartinHanak]

Hi,

I am sorry I am not able to give you any advice. I can only confirm that chamfer created after unbend will make it impossible to bend geometry back.

The question remains why you want to use the given procedure.

[hyarth]

When we bend metal sheets in factory, we cut metal sheet before bending. so I want to know the angle change  that occurs when bend with chamfering. If you know other procedure to solve this question, you can ignore my procedure.

[hyarth]

For exaple, when champered 30degree metal sheet bended, angle changed lager or smaller like 27degree or 33degree.

[MartinHanak]

Hi,

please attach a picture explaining the difference.

Note: In your previously published picture chamfers did not consume end faces of unbent sheet, therefore the sheet size with/without chamfers is the same.

[hyarth]

For example simply bending the cylinder, First, I made a cylinder with a thickness of 56 by spinning, then I made it into a flat plate by unbending.

Then, I chamfered it so that the angles were 55 degrees and 35 degrees for welding.

Third, if you bend it and remake it into a cylinder to measure the angle, the difference in angle will occur as follows. I want to do it at cone.

Here's another example

[MartinHanak · Accepted solution]

Hi,

I added two cylinders to your model (diameter=916 and diameter=1100) ... see  following picture.

For both cylinders I did following steps:

• unbend
• chamfer 50 degrees
• bend back
• sketch using bent chamfer edge

Finding no.1

When chamfer surface is bent back then it changes from planar surface to curved surface.

This is why you cannot bend a bent cone back - Creo does not know how to deform chamfer surface.

Finding no.2

If you create sketch going through chamfer edge after bend back operation, you will get your angle.

At the top (diameter=916) it is 53.5 degrees.

At the bottom (diameter=1100) it is 52.9 degrees

So you know that the angle varies between two above values. >>> and this is the answer you are looking for (I hope).

[hyarth]

Yes that's what I wanted, but if this is chamfered inside the cone, it seems that bend back is impossible.

Could this problem be solved?

[MartinHanak]

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@hyarth wrote:

Yes that's what I wanted, but if this is chamfered inside the cone, it seems that bend back is impossible.

Could this problem be solved?

---

Hi,

I opened model shown in my reply from ‎2023-02-24 02:37 PM, changed outer chamfers to inner ones and redefined Sketch features. Model was regenerated successfully. NO PROBLEM.

[hyarth]

If you don't mind, could you upload the model file? I'll open the commercial version later.

[MartinHanak]

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@hyarth wrote:

If you don't mind, could you upload the model file? I'll open the commercial version later.

---

Hi,

I am sending data.

[hyarth]

Thank you for your help!

[kdirth]

After a bit of experimentation, with a cone, it appears creo is unable to bend back a cone if you modify the end of the driving surface.

[hyarth]

cone's thickness was 50

[kdirth]

The bend back feature needs the original anchor surface, or at least a portion of it, to work.

Also, you don't need to unbend in order to chamfer the edge.

[hyarth]

Specifically, I would like to know the angle change that occurs when bending again after chamfering in the unfolded state.

[StephenW]

If you are talking about deformation due to manufacturing process, Creo is not doing that for you. Creo will calculate the "stretch" in the part from flat to form based on the given "y" or "k" value in the settings (it is your responsibility to set the correct value based on the manufacturing method and materials used). 

All Creo Parametric will do for you is calculate bend allowance. See machinery handbook or google bend allowance. It is NOT doing anything other than solving a relatively simple calcuation based on value given.

If you need more than that, you will need other analysis tools.