CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   CFX FSI simulation floating point error after 2500 steps (

munnamarfy July 15, 2013 23:22

CFX FSI simulation floating point error after 2500 steps
4 Attachment(s)
Dear Members, good day
I am solving a simple FSI problem of flow over a cantilever plate with a square obstruction. (see attached picture). after around 2720 steps I got an error as: (my error is common but I want to see experts advice about case)
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver.

In third picture I observed distorted mesh at the tip of cantilever. which first observed at around 2000 step but simulation failed at 2720 step.
Is it because of my mesh, but usually in case of extreme deformation of mesh a FOLDED MESH ERROR observed.
or due to BCs ( Used opening type BCs)?
my flow conditions are Mach 0.1 , Re = 200.
unstructured mesh. dt =0.005 sec( i also checked with dt0.001, but same error at some other point of time)

size: plate length 0.5m, square block = 5 cm side
domain size= 20m x 30m

please help me out.

stumpy July 23, 2013 16:41

If this is a repeating oscillating case, then use "Dispalcements Relative To = Initial Mesh" to avoid the mesh degrading over time.

munnamarfy July 24, 2013 02:11

Thank you Stumpy,
My plate sustained oscillations due to vortex flow. May I know exactly mean of repeating oscillation ( oscillation itself a repetition).

I am trying to locate the mentioned option 'displacement relative to initial mesh'. Can you help me to find the same.

Thank you

stumpy July 24, 2013 10:41

The setting is on the Domain > Basic Settings panel, just below where you enable the Mesh Motion model.
I see your point about repeating oscillations! Repeating motion would be a better description, so I think your case does have this. The mesh will get worse after every oscillation without this setting.

munnamarfy July 24, 2013 22:46

1 Attachment(s)
Dear Stumpy
I am running a FSI problem under workbench plate form. and in my domain panel i am not able to see "Dispalcements Relative To = Initial Mesh" option. there is only one option available as "displacement diffusion" please see attached picture. I will be highly obliged by your valuable reply.
Thank you

stumpy July 29, 2013 15:19

Are you using the most recent version? In older versions you would need to add this manually to the CCL under the MESH DEFORMATION: section:

Displacement Relative To = Initial Mesh

All times are GMT -4. The time now is 00:19.