I get different results when running the same model on different computers

19yuuki9119yuuki91 Member Posts: 8

Hi all

Like the title suggests, for some reason I get different results when running the same model on different computers, and I wanted to ask you guys for possible mistakes I could be making that I have overlooked.

To give a bit more details, I am using ANSYS 19.2 Academic Version. The model is a static analysis of a compression prism using solid65 for the brick and mortar and solid185 for loading plates. I applied a load larger than it could withstand (which was defined by trial and error in other previous analysis), and divided into the appropiate amount of substeps for my analysis. Then ran the analysis and in one computer it is able to converge up to substep 130 and in the other to substep 126, for example.

I was not sure what was going on, so I decided to create the model from zero in each computer, applied the same methodology in each one, but once again I got different results, one computer is able to converge up to a substep larger than the other. I plotted the results, and they are basically identically up to the last substeps where they differ a bit. However, given that I am running the same model, I feel they should be identical.

The computers I tried it on are:

ASUS G14, RYZEN 9 5900HS, 32 GB of RAM and a 3060 graphics card

ACER, I5-8250U, 8 GB of RAM, and a 150MX graphics card.

In any of the analysis I tried the ASUS one is always able to converge further. I hope you guy can give me an idea of what I am doing wrong.


Best regards

Comments

  • SheldonISheldonI Posts: 112Ansys Employee

    Hi @19yuuki91 ,

    You noted that the results are basically identical up to the last substep, but is cracking/crushing (material failure) occurring at the last substeps? If so, the numerically and physically unstable nature of the model may be causing this difference.

    Please see Section 4.6 "Troubleshooting" of the Parallel Performance Guide of the Mechanical APDL documentation. Specifically, a section titled "Different Results Relative to a Single Core" discusses this. When the model is numerically unstable, you can get different results if you use different # of cores or if the chip architecture is different between the two machines.

    It is not that one solution is correct but the other is incorrect - when we have numerical or physical instability, even tiny changes can affect the results or convergence pattern. While not a perfect example, consider a rubber ball being dropped vertically on a rigid surface - we may expect the rubber ball to bounce vertically back up after it hits the ground, but because of the mesh discretization and other factors, the ball may bounce to the left or to the right. There isn't a single 'correct' solution in this case - because of the unstable nature, we wouldn't say that the ball bouncing to the left after hitting the ground is 'incorrect'. When SOLID65 starts to crack/crush, the stiffness is dramatically reduced (or goes to zero), introducing numerical instability - depending on the problem setup, there could be physical instability of the crack propagates quickly.

    If, however, your model is not experiencing any cracking/crushing near the last substeps, then the difference in results or convergence pattern would be due to something else.

    Regards,

    Sheldon

  • 19yuuki9119yuuki91 Posts: 21Member

    Dear Sheldon

    I apologize for the late response. I checked the guide as you suggested, as well as the model. Like you said cracking was occurring in the late stages of analysis in my model, which could have contributed to the numerical instability and I think this is the reason for the small discrepancy between models. I checked everything else, and they seemed identical.

    Just to add a bit to the discussion, I did the same model in workbench and once again I got some discrepancy in the results at the end. This too could be accounted by the numerical instability of the model? In the convergence crfiteria of workbench, what rule is being used? In the APDL you can choose between L1, L2 and infinite, and I was a bit curious about WB since it does not seem to have an option choose.


    Thank you very much for your answer, it helped me quite a bit to clarify many doubts and confusion about my mode,


    Best regards

    Yuuki

  • SheldonISheldonI Posts: 112Ansys Employee

    Hi Yuuki,

    Sorry for my delayed response as well. :)

    Workbench uses the same default for checking Newton-Raphson residuals, which is the L2 norm. I would not change this parameter - you can tighten the criterion, if needed, but this is usually rarely needed.

    Regards,

    Sheldon

Sign In or Register to comment.