Skip to content

Troubleshooting Common Issues

"Time increment required is less than the minimum specified" — what does this mean?

Abaqus/Standard applies loads incrementally. The step time runs from 0 to 1, where a step time of 0.1 means 10% of the total load has been applied. At each increment, the solver checks for equilibrium. If equilibrium cannot be found, it cuts the time increment and tries again with a smaller load step.

This error means the solver has cut the increment so many times that it hit the minimum allowed size and gave up. It is a sign of non-convergence.

Things to try (one at a time):

  1. Check all inputs — material properties, unit consistency, load magnitudes, and boundary conditions. Many convergence problems are caused by incorrect inputs.

  2. Visualize partial results — open the .odb file even if the job did not finish. Look for contact penetration, unexpected large displacements, or buckling behavior that may explain why the solver is struggling.

  3. Increase the maximum number of increments and/or decrease the minimum increment size: In the Step Module, open the Step Manager, select your load step, and click Edit. Go to the Time Incrementation tab and increase the maximum increments (e.g., 200) and/or decrease the minimum increment size (e.g., 1E-10).

  4. Allow more cutbacks: Go to Tools > General Solution Controls > Manager, select the load step, click Edit, then Continue. Under the Time Incrementation > More tab, increase the value of I_A (the allowed number of cutbacks per increment, e.g., 20).

  5. Add automatic stabilization: In the Step Manager, edit your load step. Under Automatic stabilization, select Specify dissipated energy fraction and leave the default value. This allows a small amount of artificial energy dissipation to help the solver through difficult increments.

!!! note Abaqus/Explicit uses time steps that represent actual time and is intended for dynamic analysis. The step time behavior described above applies to Abaqus/Standard only.

How do I fix issues with an imported part?

Geometry imported from CAD (e.g., SolidWorks) sometimes causes problems in Abaqus due to small edges, redundant faces, or complex lofted features.

Steps to try:

  1. Simplify the part in SolidWorks before exporting — especially lofts and other complex construction features.

  2. Export as ACIS (.sat): In SolidWorks, click Save As…, select Options, and ensure the version is 22.0 with the correct units selected.

  3. Try alternative file formats if .sat doesn't work:

  4. .SLDPRT (for newer versions of Abaqus)
  5. .VDA (imports in mm — scale in the Import dialog to get inches)

  6. STEP AP203

  7. Clean up the imported geometry in Abaqus: In the Part Module, use Geometry Edit:

  8. Edge > Remove redundant entities — box-select the entire part to remove extra edges created by plane intersections in SolidWorks
  9. Edge > Remove small — removes tiny slivers that can cause mesh failures
  10. Face > Remove — useful if a protruding face needs to be eliminated (you may need to partition the part first)

My model is running but the results look wrong — where do I start?

Work through this checklist:

  1. Units — Abaqus has no built-in unit system. Confirm that your length, force, mass, and time units are all consistent throughout (material properties, loads, geometry, and density).

  2. Boundary conditions — Are the supports constraining the right degrees of freedom? A free model or an over-constrained model will both give wrong answers.

  3. Material properties — Double-check elastic modulus, Poisson's ratio, and (for vibration) density. Density is a common source of error — see the Vibration Analysis page for unit conversion details.

  4. Reaction forces — Run the model and check that the reaction forces at your supports sum to the applied loads. If they don't match, something is wrong with your loading or BC setup.

  5. Compare to a hand calculation — Even a rough estimate from beam theory or plate equations will tell you if you are in the right ballpark.