Creo 3: I have been having an issue with suppressing or clip suppressing instance features. I have a Generic Part and am changing dimensional values by using a Family Table. I open an instance and there is a feature that fails. I choose Clip/Suppress, the prompt to access (Yes/No) appears and I select Yes to continue. The same failed feature keeps repeating and I cannot get out of it. See below.
Feature 59 of an instance fails because I changed a dim. It is a surf to surf round.
I select Quick Fix>Clip/Suppress, the prompt "Yes/No" appears and I select "Yes". Creo loops and displays Feature 59 failed. It is a never ending loop. I have not been able to find a solution.
Not a real fix but you might see if precision is failing the feature.
Otherwise you will need to find a robust way to manage this feature.
I suspect the Clip/Suppress option is only temporary.
This needs to be addressed at the geometry level.
You could use relations that make sure that only valid values can be used.
The solution is to choose "Quick Fix>Delete". Delete does not delete the feature in the Generic and only adds the feature with "N" to the Family Table. Now the feature can be changed in the Generic or the dimensional value can be added to the family table to allow it to regenerate properly.
The following appears in the Family Table after choosing "Delete":
Our CAD Standards do not allow us to change the Accuracy of parts. We must use Absolute Accuracy of .004. I do not know why someone determined we cannot change accuracy of parts except in the past the higher accuracy caused longer time to regenerate parts. With today's computing power I do not think an accuracy change that allows parts to regenerate properly would be any issue/concern at all?
Accuracy changes can cause failures in merge/inheritance features, if you use them. I generally agree that you should not change the accuracy, but I don't agree that it should be "not allowed".