Sheetmetal: Inside diameter changes when thickness is changed

[NK_7184747]

I have encountered an issue that I cannot seem to solve, when working with sheetmetal parts.

The sheetmetal part has different features to be placed 360 degrees around a cylindrical object, for laser engraving purposes. So the thickness of the sheetetal is on paper irrelevant - so ideally so thin it is just visible on the assembly.

The dimensions of the sheetmetal part matches the diameter of the object and so does the features on it - atleast theoretically. The sheetmetal bend is set to 360 degrees and to keep the dimensions on the inside of the bend.

But, when assembling the sheetmetal with the cylindrical object, I get small inaccuracies on the technical drawing of the assembly - the angles between the features do no longer match, which is an issue on the given task.

I have found out that changing the thickness of the sheetmetal impacts the position of the features, even though the part is set to keep the dimensions on the inside of the bend, and I do not know why.

I am working in Creo 7.

Can anyone help me on what I am doing wrong or how to find a solution? Thanks.

[StephenW]

First thoughts, parts that touch in an assembly can cause visual discrepancies on a drawing.

Really thin parts can also have visual issues. 

Accuracy setting on component could also be an issue here.

accuracy on the part can be looked at under File - Prepare - Model Properties. 

BEFORE MAKING ACCURACY CHANGES, SAVE YOUR FILE!

If accuracy is set to relative, you may want to consider switching to absolute accuracy. Making the relative or absolute accuracy smaller may help.

You may also need to change the accuracy of the assembly.

Changing accuracy affects regeneration time on large models and can cause unexpected consequences. Don't save until you review your model.

[tbraxton]

"I have found out that changing the thickness of the sheetmetal impacts the position of the features, even though the part is set to keep the dimensions on the inside of the bend, and I do not know why."

What observations leads you to this conclusion? Queries of dimensions in part/assembly mode or changes to dimensions seen on a drawing? If drawing dims, how did you create the dimensions in question on the drawing?

More information is needed, post the models and more detail on what is happening when the thickness of the part is modified.

[kdirth]

Is the final design intent to show the laser engraving on the surface?  Would using Designate Area accomplish the required result?

Wrap a sketch around the cylinder and designate areas to be engraved.

[anursingh]

Hi @NK_7184747,

I wanted to follow up with you on your post to see if your question has been answered. 
If so, please mark the appropriate reply as the Accepted Solution. 
Of course, if you have more to share on your issue, please let the Community know so that we can continue to help you. 

Thanks,
Anurag

[NK_7184747 · Accepted solution]

Hi Anurag, yes sorry for not having followed up myself earlier.

I did not find the solution to my specific problem in the suggestions, even though they were helpful to understand other things in Creo.

In the settings used by the engineers creating the parts (years ago), they had applied a default K-factor on the sheetmetal 'bend' feature - even though the part was not intended to have, bend back, stretching etc..

This was not obvious to me in the first place, since I had not worked with sheetmetal before in Creo.

So after instead inputting a K-factor manually to '0', I could adjust the compensations already made to the part and start using the theoretical values instead.