A couple of times recently, I think I've had an issue whereby a relation that produces a non-rational value and assigns it to a dimension causes the regen status to remain yellow - presumably because the dimension precision immediately changes the dimension value to be unequal to the result of the relation.
To give a specific example: I'm getting the error "Some relations are no longer satisfied in 00929329 for SD5."
The relation is
sd5 = 90/nom_teeth
where nom_teeth = 21, therefore
sd5 = 4.2857142857142857142857142857143.
My guess is that the the value of sd5 is then rounded to 4.286, and
4.286 != 4.2857142857142857142857142857143
therefore the relation is "no longer satisfied".
How do I stop it worrying about this, and get a green regen status?
WF5 / CEP / Creo 0 on this particular project.
Typically this message means that after two successive regenerations, something is still out of date. Easy way to see if it's a decimal precision issue, round the number down (or up) to a specified number of decimal places.
sd5 = FLOOR((90/nom_teeth),3)
Thanks, Tom - that showed that it wasn't a decimal issue.
On further digging... sd5 had been changed to (rsd5) - and yet there was no error message telling me that the relation was now trying to change a reference dimensions!
Another quality piece of PTC error reporting...
replace section relation with the appropriate part relation. If you do this step then all relations will be defined on the same level. I hope that this helps you to find the cause of the problem.
I have not had any issues with this. The value is still 13 places including both sides of the decimal place. You can look at the properties of SD5 (whatever the symbol is after the sketch is closed), and you will see it rounds display, but the value is still 4.285714285714 (or close to it).
The only time I found Creo rounding a calculation value is in the tab dialogs. You have to go back and edit the associated dimension property to get it to a finer precision by entering the fractional value again. This is very problematic to me but if you are aware, it is manageable.
I'm going to suggest there is another issue here that has the sketch trying to do something it doesn't want to do. I have had nothing but trouble with angles when it comes to reaching 0 degrees. It just cannot quite get there. but if you change the references to be equivalent at say 90 degrees, it has no trouble whatsoever. I run into this over and over again and just cannot quite capture it for a bug report. I know R&D has got to be aware of it as it is quite pervasive.