

August 27, 2019 at 3:28 pmbermetkerimkyzySubscriber
Hi everyone,
I'm trying to simulate creep on a simple rectangular plate subjected to tensile stress. I'm modeling a quarter of the geometry (with pressure applied on one edge and 2 other edges with symmetry BC).
I'm using a polymeric material, for the creep law I chose Norton's equation with coefficients known.
When running the simulation I'm having the following error:
Error Message: The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information
Can you help me with this? Please see the model in the attachments.
thank you!
/Bermet

August 27, 2019 at 7:11 pmpeteroznewmanSubscriber
I looked at your model. One mistake in the model is in the Symmetry Normal.
In Symmetry Region, which is the line along the Y axis, you have the Normal as the Y axis, change that to X axis.
In Symmetry Region 2, which is the line along the X axis, you have the Normal as the X axis, change that to Y axis.
Under Analysis Settings, set Large Deflection to On and the Solver Type to Direct.
As a diagnostic test of the model, I reduced the Pressure to 1000 Pa and set step 1 to end at 0.1 s.
The model converges step 1, which is progress. I now have a uniform normal Y stress of 1000 Pa.
If you plug that stress into the Norton equation with the coefficients you provided, you get a strain rate of 1.253*10^3
For Load Step 2, I changed the end time to 1 second. I changed the Initial Substeps to 10^5, the Minimum Substeps to 1 and the Maximum Substeps to 10^6.
The model runs from 0.1 to 0.364 s when the material stretches from the 0.1 m long original length to 18 m long!
I recommend you reduce your pressure to a much smaller value.

August 27, 2019 at 7:55 pmbermetkerimkyzySubscriber
Thank you! I retried with your suggestions. Now the model is running without errors, thank you! The mistake with coefficients was that I calculated them for stress in MPa, so now I have put my pressure and Young's modulus in MPa.
However, I have a problem with the output data. The values of stress and strain are not as they should be during the creep. The stress is not relaxing and the strain shows not the power law behavior but linear!
What is the error? I attach the updated model in the original post (creep_trial_plate2)
Thank you.

August 27, 2019 at 8:18 pmpeteroznewmanSubscriber
I looked at the Young's Modulus in your original file and it seemed to be of the right order of magnitude.
The Young's Modulus you have used is the wrong order of magnitude. It can't be 6000 Pa. You had it right the first time.
You have the Norton Creep coefficients to use Units of N and m = Pa, so that must match your Solver Units.
In the second model, you forgot to change Large Deflection to On under Analysis Settings.
Since you have a constant pressure, the stress will not relax. The graphs that you show above are correct. To see stress relaxation, you have to stop pulling and fix the displacement instead.

August 27, 2019 at 9:48 pmbermetkerimkyzySubscriber
yes, I thought I could get around by simply pretending N/m2=MPa, but that you're right, I should use the correct units and recalculate the coefficients in correct units.
regarding the stress relaxation, I think I'm lacking here basic understanding of how the software works. I switched now to displacement that is equivalent to my constant pressure value and now everything works fine.
thank you a lot for the help!
/Bermet

 You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Saving & sharing of Working project files in .wbpz format
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 Solver Pivot Warning in Beam Element Model
 Colors and Mesh Display
 whether have the difference between using contact and target bodies
 How to calculate the residual stress on a coating by Vickers indentation?
 What is the difference between bonded contact region and fixed joint
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 User manual

2678

2120

1349

1136

461
© 2023 Copyright ANSYS, Inc. All rights reserved.