Thermal & structural analysis on Ansys workbench 18.2

  • Last Post 09 October 2018
  • Topic Is Solved
HAB! posted this 07 October 2018

I am having an error stating that " An unknown error occurred during solution. check the Solver Output on the Solution Information object for possible causes".

I am doing Thermal & Structural analysis on the rocket nozzle. Thermal analysis is successful but structural analysis is showing this error. I am using Ansys workbench 18.2. Can you help me through this?


Order By: Standard | Newest | Votes
HAB! posted this 08 October 2018

Hi peteroznewman,

I performed transient structural analysis again, this time I did not applied pressure loads. After thermal analysis I performed following steps:

1) edited the material property to include the structural property of 4 materials I am using in the project

2) I imported the body temperature

3) I added fixed support

4) filled the analysis setting 

after that I solved it. But it failed again. and following errors are coming up:

1) Element 1663 located in Body "SP-1" (and maybe other elements) has become highly distorted.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere.  Try incrementing the load more slowly (increase the number of substeps or decrease the time step size).  You may need to improve your mesh to obtain elements with better aspect ratios.  Also consider the behavior of materials, contact pairs, and/or constraint equations.  If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object.

2) The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

3) The maximum contact stiffness is too big. This may affect the accuracy of the results. You may need to scale the force unit in the model.

I am using 4 materials named as: Carbon phenolic, Silica phenolis, graphite and steel

Can you please help me through this, since my thesis deadline is few days from now. 




peteroznewman posted this 08 October 2018

Hi HAB!,

Is the fixed support a correct way to model this structure? A fixed support is a problem when you have a large thermal expansion happening if that does not accurately represent the boundary conditions. This is a rocket nozzle connected to another part of the rocket. You have to model a long enough part of the structure to capture the temperature going from very hot to ambient. Are you using symmetry in the model?  Please post some screen snapshots of the model.

You can create a named selection to see where the distorted element is in the model. Is it near the Fixed Support?  If so, the solution may be to change from a Fixed Support to three displacement constraints that allow the nozzle to expand without picking up stress from the displacement constraints.

Do any of the materials have plasticity or other nonlinear behavior?  If so, you may need to use Substeps to take smaller load increments.

You can change the Contact Stiffness to get rid of that warning.

Please create a Workbench Project Archive and attach that after you post your reply.


HAB! posted this 08 October 2018

Hi, I have deleted all my messages. Thanks a lot Peter. I really appreciate it. I’ll wait for your feedback. Thanks

peteroznewman posted this 08 October 2018

This model is a small angular slice from a full revolved solid. As such, it should have Symmetry conditions on the cut faces in the Transient Structural analysis.

What is the face that is fixed connected to that is holding it fixed?  I think a better constraint is to apply a displacement of X=0 to the flat face. That combined with two symmetry conditions can replace the fixed support.

HAB! posted this 08 October 2018

The face that is normally fixed with the engine assembly is the vertical face of the convergent part and the portion of the steel structure which I previously showed through Snapshot that represented fixed support. I can try giving displacement=0, but can you please give little more detail about symmetric condition on the cut faces? Thanks.

peteroznewman posted this 08 October 2018

Fixed support at just one end defined a long cantilevered structure which doesn't represent the physics of the real part. Replace fixed support with a zero displacement on three faces, the two cut faces and the flat base.

I added a Modal Analysis so you can see the the effect of the three displacement supports. I suppressed the Fixed Support. But if you suppress the three displacements and unsuppress the fixed support, you can see in the Mode Shapes the freedom that the fixed support allows is too great and does not at all represent how this slice works with the rest of the nozzle. The displacement supports allow the nozzle to expand radially outward with the thermal temperature because the nodes are allowed to slide in the plane of the cut. But the displacement supports on the cut also support the pressure load by allowing hoop stress to build up in the nozzle.  With just a fixed support, those pressure loads were trying to bend a cantilevered beam instead of stretch a revolved solid.


That lets the Transient Structural solve, at least for the first 0.8 seconds, when I stopped the solution so I could archive it and send it back to you.

Attached is an ANSYS 18.2 archive.


Attached Files

  • Liked by
  • HAB!
HAB! posted this 09 October 2018

Hi Peter,

This is amazing. Thanks very much. Its a big load off.