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

FSI Thermal energy non-convergence...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 24, 2010, 21:39
Default FSI Thermal energy non-convergence...
  #1
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Dear all,

I performed an FSI, and it resulted to a Thermal energy non-convergence, T-Energy did not converged to my required residual. on the T-Energy plot, it was going towards convergence until after the 153rd iteration and it remained in a state of oscillation with lots of high frequency peaks.

how should i go about diagnosing my results/setup please?

look forward to hear of any comments/suggestions. Thanks!
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 26, 2010, 17:15
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you turn FSI off does it converge quickly?
ghorrocks is online now   Reply With Quote

Old   January 26, 2010, 20:58
Default
  #3
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi Glenn, thanks for your reply.

i would like to perform a fluid-solid heat transfer using FSI. if i were to turn FSI off, will it not calculate the heat transfer properly please?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 26, 2010, 21:07
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX can do fluid-solid heat transfer itself with no need for FSI. Why are you using ANSYS for the heat transfer? What is stopping you doing everything in CFX?
ghorrocks is online now   Reply With Quote

Old   January 26, 2010, 21:58
Default
  #5
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
So sorry Glenn, i'm confused...

i am calculating heat transfer totally in CFX..... the solid model and fluid model are in CFX. i've created the Fluid Solid Interface sides in CFX......

are you asking me to delete the Fluid Solid Interface sides in CFX and CFX will still calculate heat transfer for me??? what do you mean by turning off FSI please?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 26, 2010, 22:02
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
OK, in that case you are not doing FSI, you are doing a conjugate heat transfer simulation or CHT.

Can you describe what you are modelling?
ghorrocks is online now   Reply With Quote

Old   January 26, 2010, 22:26
Default
  #7
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
i'm modeling heat transfer from a housing (cylindrical in shape) which has coolant ports, one inlet & one outlet. heat source is heat flux from the inner surface of the housing. i would like to calculate the pressure difference of the cooling channel design, heat taken away by coolant and film coefficient.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 26, 2010, 22:55
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Is the fluid coupled to the heat transfer? If so, how? When you run the fluid by itself does it converge?
ghorrocks is online now   Reply With Quote

Old   January 26, 2010, 23:06
Default
  #9
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
I mainly followed most of the setup in the CHT tutorial...
Both fluid & solid model Heat transfer setting is Thermal Energy.
fluid solid interface mesh connectio method is GGI
Fluid has finer mesh than solid.

All other RMS residuals (P-Mass,U-Mom,V-Mom,H-Energy,E-Diss.K,K-TurbKE) converged to my set residual target, EXCEPT for the T-Energy.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 26, 2010, 23:15
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you worked through the issues discussed here:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Are you steady state or transient?

With CHT a number of other issues come up. The main one usually is the fact the solid time scales are much slower than fluid time scales, which results in the fluids converging normally but the solid converging very slowly. If you are doing a steady state run the fix for this is to use the solid timescale factor to run the solid at a faster rate to the fluid. If transient you just have to be patient and wait for it to finish!

But you are not getting slow convergence you are getting a failure to converge. This may still be fixed using solid timescale factors, but can also be caused by many other factors.
ghorrocks is online now   Reply With Quote

Old   January 27, 2010, 00:27
Default
  #11
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
i'm performing a steady-state analysis.

i've set the Solid Timescale Control > Solid Timescale = 2[s].
for the fluid Timescale, it is set to Auto Timescale. From the results file's Timescale information table, the Fluild timescale has always been 9.7e-2
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 27, 2010, 00:45
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Try making the solid timescale 100x larger and as a second test the same as the fluid time scale.
ghorrocks is online now   Reply With Quote

Old   January 27, 2010, 02:12
Default
  #13
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi Glenn,

For Steady-state, one of the fix mentioned above is to use the solid timescale factor. To run the solid at faster rate, should i increase the solid timescale factor? is it the same effect as reducing the solid timescale??

i'm also attaching a picture file of the T-Energy convergence graph. It is not converging slower than the fluid, but not converging at all......
Attached Images
File Type: jpg T-energyNonconvergence.jpg (36.2 KB, 20 views)
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 27, 2010, 16:49
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The solid timescale factor is the factor by which the solid time scale is larger than the fluid timescale. 100 means the solid timescale is 100 times the fluid timescale.

Have you looked at the residuals in CFD-Post? That will tell you where the problem residuals lie. You will have to put the residuals in the output file.

Can you post the CCL of your simulation?
ghorrocks is online now   Reply With Quote

Old   January 28, 2010, 15:45
Default
  #15
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
Turn on double-precision too.
stumpy is offline   Reply With Quote

Old   January 29, 2010, 00:58
Default
  #16
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
To Glenn:
i didn't put the residual into the output file to view it in CFX-Post...... could i edit the result file and export the residual or should i redo the calculation again with the output setting to include residuals please?

To stumpy:
where do i turn-on the double precision please? does this require me to redo the calculation please?

attached also is the CCL file.
Attached Files
File Type: txt convergence prob.ccl.txt (24.4 KB, 7 views)
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   January 29, 2010, 17:47
Default
  #17
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
See the doc for double precision. Also, if you have a matching mesh at the fluid-solid domain interface, change the interface so the mesh connection method is GGI. If it's non-matching it will be GGI in any case.
Regards
stumpy is offline   Reply With Quote

Old   January 30, 2010, 06:45
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You will need to rerun to put the residuals in the output file. Don't forget this just needs to be a restart, so no need to go right from initial conditions.

Stumpy's suggests are also worth trying. Have you tried double precision and forcing use of a GGI?
ghorrocks is online now   Reply With Quote

Old   February 2, 2010, 23:31
Default
  #19
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi guys,

I've forced to use GGI meshing from the start. but not double precision....... i still can't find how to set this double precision in CFX-Pre... any directions please?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   February 3, 2010, 04:58
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
In V11 you need to select double precision in solver manager or the command line. In V12 you can select it in CFX-Pre.
ghorrocks is online now   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
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
Diff bet total energy & thermal energy model?? vijeshjoshi23 CFX 5 October 9, 2009 10:31
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
SIMPLE and energy equation convergence Fabio Main CFD Forum 0 June 1, 2007 06:06
Info: Short Course On Thermal Design of Electronic Equipment Arnold Free Main CFD Forum 0 August 10, 1999 10:18


All times are GMT -4. The time now is 02:33.