Announcement

Collapse
No announcement yet.

time steps

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • time steps

    image.png


    What does 'time steps' mean here? Does 'static' mean 'stationary analysis' or 'time transient analysis'?

  • #2
    Hi emB,

    The difference between static and dynamic analysis is the absence in the former and inclusion in the latter of inertial terms. In either case, FEBio will step through time given the number of time steps and the time step size.

    Even for a static analysis, it can be beneficial and sometimes necessary to apply loads incrementally through time. Loads can be ramped up through time via load curves and FEBio Studio will often automatically attach load curves to the parameters of loads and prescribed displacements. You can find these curves in the Curve Editor (menu Tools\Curve Editor).

    If you really want a single-step static analysis, then you can set the time steps to 1 and the step size to 1 as well.

    Finally, if your problem is not intrinsically time dependent (e.g. the material is elastic), then the units of time won't matter. However, for models that are time-dependent (e.g. it has viscoelastic materials) the time units do matter, and you have to ensure that the "step size" is in the correct units.

    Let me know if you have further questions about this.

    Best,

    Steve

    Department of Bioengineering, University of Utah
    Scientific Computing and Imaging institute, University of Utah

    Comment


    • #3
      Hi steve, thank you for your reply!

      I don't really understand why time doesn't matter when i use elastic material.

      https://drive.google.com/drive/folde...Hn?usp=sharing

      this is my model and i tested different 'Time settings' under the same boundary condition. Different stress values appeared in different timelines, how do i know it's converges or not

      Comment


      • #4
        Hi emB

        Just to clarify, I was only commenting on the units of time. Even for elastic materials, you can build a time dependency into your model (e.g. by assigning load curves to loads, boundary conditions, or even material parameters), so whether time matters, depends on more than the choice of material.

        Regarding your model, there are no loads, just contact with an initial overlap. In theory, your model should converge in a single step, regardless of the step size. I ran the first case, and the model converges indeed in a single time step. The reason why the remaining steps continue is because augmented lagrangian is on, which continues to try to crank up the contact pressures, but the increments become smaller and smaller.

        I don't know what the stress values that you report in that excell document mean (are they taken from a particular location?), so I can't comment on that. I looked at the peak effective stress and it remains constant after the first timestep. If you can explain what these numbers mean, then I'll take a closer look on my end.

        Best,

        Steve
        Department of Bioengineering, University of Utah
        Scientific Computing and Imaging institute, University of Utah

        Comment


        • #5
          Hi Steve

          I apologize for the lack of explanation. There are two geometry in my model, upper and lower. and i need both of upper's stress and lower's stress. What you looked at the peak effective stress is lower's peak effective stress, and I report in that excell document is upper's peak effective stress.

          And I am comparing these stresses with the analysis results of comsol. Based on upper, FEBio's Effective stress is 0.34[MPa] in a first time step, 0.75[MPa] in a 500th time step, Comsol's Von Mises stress is 0.73[MPa] with same fixed displacement, contact pair and used stationary analysis.

          Please let me know if my explanation is still lacking.

          Comment


          • #6
            Thank you for that explanation.
            I took a closer look at the lower part, and I do see the effect that you noticed now. As I mentioned, the augmented-Lagrangian will continue to crank up the contact force in repeated time steps. When you see that the contact force continues to change, it might be an indication that the convergence criteria on the augmented Lagrangian are set too loose. Therefore, you could crank up the convergence criteria, or on the other hand, you can just do what you are doing and run more time steps. You can monitor the peak effective stress to see whether the solution eventually converges. I guess this is one exception to the rule above, where even when all things stay the change, the results can still change with increased number of time steps.

            I'm glad to see that (eventually) the febio results do seem to agree well with Comsol's.

            However, even when the augmented Lagrangian eventually converges, I would still be cautious about accepting the results. The contact appears to be very localized in one particular spot. It seems that the edge of the upper part is barely grazing the lower part. With the mesh being so course in this area, I'm not sure the results are mesh-converged. I would consider making a more refined mesh, especially in the areas of contact to see if you can resolve that contact better. It might have a significant effect on the peak-stress.

            Best,

            Steve
            Department of Bioengineering, University of Utah
            Scientific Computing and Imaging institute, University of Utah

            Comment


            • #7
              Hi Steve.

              Thank you so much for your valuable inputs. I will definitely work on the suggestions you've given.

              Comment

              Working...
              X