Static structural model solves in Mechanical 2023 but not in Mechanical 2024

[mergen.eric]

Hi,

I have a static structural analysis model that solves in Mechanical 2023, but won't solve in Mechanical 2024. The Solver Information has an Error section and Fatal section. I've attached a screen capture showing the details. Any idea why the analysis would solve in an older version of Mechanical but give errors in a newer version? 

 

[Akshay Singh]

Hi,

It is likely that the program controlled behavior of certain connections have changed from one version to another.

Please compare the .dat files of the two versions to check the difference in keyopts or other such properties/settings bewteen the two versions.

dat files can be found under Solution > Right click>solver Files directory

copy the dat files of the two versions to a new location. Rename them appropriately. eg. dat_v232 and dat_v242
Use a text comparison tool to check the difference bwteeen the two files and take necessary action-->for instance changing the program controlled beahvior to match with the working model

[Dennis Chen]

I know exactly what happened here:   In 24R1 or so, Ansys changed the default contact formulation from augmented lagrange to MPC.   This is why you are having this issue.   Look at all of your contact and if you have any default contact formulation (proramm controlled), change them to augmented lagrange and your model should solve.

I was working at a Channel partner at the time and I had a lot of personal complaints about this.   Program control looked like a great idea but in reality, it is just hiding important modelling decisions from the user.   If there needs to be a default, specifically state what the default is, there's 0 value in having an option named "program controlled".   If we all think about it, what does "program controlled" really accomplish other than hiding something important.

This is espeically true if you change what "Program controlled" means.