10-Marble

Question

Sheetmetal round/chamfer merges adjacent flanges

Forum|Forum|3 years ago
August 12, 2022
4 replies
3147 views

Hi everyone,

I am having some trouble after recently updating from Creo 6 to Creo 8. As far as I remember this was never a problem in Creo 6, but I don't know if there could be some difference in a config/bug arising as a result of my organisition's specific distribution.

Problem:

I am creating a sheet metal part with two overlapping flanges whose flat faces 'meet' to create a more sturdy fixing point when riveting the part in place. The position of one bend is offset by the thickness of the material to create the overlap without the flanges actually intersecting. I would like to apply a round to the corners, however this causes a big problem. When the round (or chamfer) are applied across the two independent corners the resultant geometry instead creates a single franken-flange by merging the two at the round. The image below shows the part I am working with. The two bends are numbered, while the problem area is marked with 'P'. The two flanges still highlight individually if selected via the model tree, but otherwise the flat edges are continuous, as if created from a single solid flange. If I then try to create an extrude cut in the affected franken-flange it's treated as a single solid body, with the 'up to next' option cutting through the whole model rather than a single original flange. This problem also results in me not being able to create a flat for manufacturing, as it throws up an error instead.

Does anyone have any experience with this? I have looked through the settings of the round function, but could not see any mention of a merge setting. Perhaps there is a config option for this? Or could this be a bug?

Workarounds:

As far as I have tested the only ways to get around this problem are to:

1) Create two separate round operations, one for the inner flange, and one for the outer. This preserves the two individual flanges, but creating two sets within the same round operation will not.

2) Add the round operation after an unbend operation, thereby separating the affected edges/faces.

Sheet Metal Design

tbraxton

22-Sapphire II

Open a part created in Creo 6 or earlier with this same scenario with the round feature in Creo 8. Regenerate all features in this model to test if the round regenerates “correctly”, if it does not then you should open a call with PTC.

If the behavior is different from Creo 6, I would look into how bodies (multi body was not present in Creo 6) are handled in sheet metal mode. When you are selecting the edges for the round, use query select function to make sure the edge selection is not the cause of the unwanted result.

mkajdan

14-Alexandrite

I can confirm this behavior in Creo 8 and also in Creo 4 so it may not pertain to "bodies". You should open a call to PTC.

No change in behavior when opening a session of Creo 8 with no config options changed.

Creo 4

Creo 8, 1 radius

Creo 8, 2 radii

N

Nairn

Author

10-Marble

Thank you very much for testing this. I couldn't end up finding a part with the same setup from a previous version to regenerate in Creo8, I think in all of the previous cases where I've used this double flange setup the edges must have been offset, rather than the corners lining up, so I wouldn't have had the problem. I will bring this up to PTC. The only way I know how to reach them is the idea forum; is there a better way to get in contact with bugs like this?

M

MartinHanak

24-Ruby III

@Nairn wrote:

Thank you very much for testing this. I couldn't end up finding a part with the same setup from a previous version to regenerate in Creo8, I think in all of the previous cases where I've used this double flange setup the edges must have been offset, rather than the corners lining up, so I wouldn't have had the problem. I will bring this up to PTC. The only way I know how to reach them is the idea forum; is there a better way to get in contact with bugs like this?

Hi,

if you need to contact PTC Support, please start at https://support.ptc.com/apps/case_logger_viewer/cs/auth/ssl/log page.

mkajdan

14-Alexandrite

If you add the round as two separate features, it behaves as expected. Still might want to put a call in.

Edit:

I guess I should have read your post more closely as you had already mentioned this.

R

RK_10338746

3-Newcomer

Hi @Nairn

To address your issue I have raised PTC case and PTC has been filed software bug (SPR) to their R&D with HIGH severity.
Please find the below article for same.
https://www.ptc.com/en/support/article/CS374918