CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

CFX FSI simulation floating point error after 2500 steps

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 15, 2013, 23:22
Default CFX FSI simulation floating point error after 2500 steps
  #1
New Member
 
Ashish purohit
Join Date: Jan 2011
Posts: 3
Rep Power: 6
munnamarfy is on a distinguished road
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.
Attached Images
File Type: jpg 1.jpg (28.4 KB, 16 views)
File Type: jpg 2.jpg (28.2 KB, 11 views)
File Type: jpg 3.jpg (38.1 KB, 14 views)
File Type: jpg mesh.jpg (98.8 KB, 9 views)

Last edited by munnamarfy; July 15, 2013 at 23:26. Reason: missed some of the text.
munnamarfy is offline   Reply With Quote

Old   July 23, 2013, 16:41
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
If this is a repeating oscillating case, then use "Dispalcements Relative To = Initial Mesh" to avoid the mesh degrading over time.
stumpy is offline   Reply With Quote

Old   July 24, 2013, 02:11
Default
  #3
New Member
 
Ashish purohit
Join Date: Jan 2011
Posts: 3
Rep Power: 6
munnamarfy is on a distinguished road
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
munnamarfy is offline   Reply With Quote

Old   July 24, 2013, 10:41
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   July 24, 2013, 22:46
Default
  #5
New Member
 
Ashish purohit
Join Date: Jan 2011
Posts: 3
Rep Power: 6
munnamarfy is on a distinguished road
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
Attached Images
File Type: jpg Mesh motion model.jpg (96.4 KB, 9 views)
munnamarfy is offline   Reply With Quote

Old   July 29, 2013, 15:19
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
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:

FLOW:
DOMAIN:
DOMAIN MODELS:
MESH DEFORMATION:
Displacement Relative To = Initial Mesh
END
END
END
END
stumpy is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to define to right point for locationInMesh Mirage12 OpenFOAM Native Meshers: snappyHexMesh and Others 4 April 10, 2014 10:12
Rigid body motion error when restarting a terminated FSI simulation lingdeer ANSYS 1 May 19, 2013 01:40
CFX error, Floating point exception Riyaz Main CFD Forum 0 November 14, 2008 07:30
cfx does not give time steps in cfxpost.why.urgent prakash CFX 2 November 24, 2005 00:06
FSI using CFX and ANSYS Bi Chang CFX 2 May 10, 2005 04:47


All times are GMT -4. The time now is 09:25.