General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Ansys Workbench_Standalone_TimeStep Error

    • JRooney


      My model in the Autodyn Standalone program has had issues for the past couple of days. I have not been able to run my analysis further due to a "time-step too small" error. Is there anyway I can fix this in the Standalone version. I cannot run the model fully without bypassing the time-step error.

      In addition I have tried to use Ansys Workbench to run my model and I cannot place a fixed boundary condition on the second level of my "column" model. I have set boundary conditions at the base of my column, and it transfers to Autodyn perfectly, but the second row of my column does not transfer to Autodyn and I cannot apply the boundary condition. Is there another way to apply boundary conditions on the second row with either nodal points or edges (or another method)?


      Please any help you can give I would really appreciate it.


      Thank you for your time.

    • Missy Ji
      Ansys Employee

      In ANSYS Explicit "Analysis settings", Step controls section, there is a field called "minimum time step", this is the minimum time step allowed in the Explicit analysis, If set to Program Controlled, the value will be chosen as 1/10th the initial time step. If the current time drops below this value the analysis will stop. 


      You can always decrease the minimum time step to continue the calculation. After loading your problem, go to "Analysis settings", select Timestep Options. Change the Minimum Time Step to a very small number, for example, 1e-15, your simulation will continue with the small time step. And the simulaiton might take a long time to the completion.


      The variables affecting the time step are the smallest cell size, gap size, velocity, and sound speed. For Lagrangian type parts, you need to examine the geometry of the parts to see if there are distorted cells.



      For Lagrangian type parts, you need to examine the geometry of the parts to see if there are distorted cells. So when you say the error messages, examine the time step contours, find out where are the distorted elements, get a better mesh quality might help increase the time step. To have timestep plotted from the graphics area, you can insert an user defined results, (see attached image), use the expression "TIMESTEP" to request timestep contours, then you could have an idea on where those small time step occurs.


      Mass scaling is another way to improve the time steps.


      I would suggest to have a uniform and good quality mesh to start. However, during the projectile impact problems, there would be distorted elements, they will not provide stiffness to the simulation, so you could also remove those elements away from the calculation by using erosion, there are multiple criterias to remove elements, you can set them from Analysis settings, Erosion controls section, you can use material failure, geometric strain limit to remove highly distorted elements.



      Erosion is a numerical mechanism for the automatic removal (deletion) of elements during a simulation. 

      • Removes very distorted elements before they become inverted (degenerate). 

      • Ensures time step remains reasonably large.

      • Ensures solutions can continue to the End Time. 

      • Can be used to allow simulation of material fracture, cutting and penetration.

    • JRooney


      Thank you so much I will look into this and hopefully be able to run my analysis, and not run into any more errors.

Viewing 2 reply threads
  • You must be logged in to reply to this topic.