CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   FSI Thermal energy non-convergence... (

mactech001 January 24, 2010 21:39

FSI Thermal energy non-convergence...
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!

ghorrocks January 26, 2010 17:15

If you turn FSI off does it converge quickly?

mactech001 January 26, 2010 20:58

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?

ghorrocks January 26, 2010 21:07

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?

mactech001 January 26, 2010 21:58

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?

ghorrocks January 26, 2010 22:02

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?

mactech001 January 26, 2010 22:26

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.

ghorrocks January 26, 2010 22:55

Is the fluid coupled to the heat transfer? If so, how? When you run the fluid by itself does it converge?

mactech001 January 26, 2010 23:06

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.

ghorrocks January 26, 2010 23:15

Have you worked through the issues discussed here:

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.

mactech001 January 27, 2010 00:27

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

ghorrocks January 27, 2010 00:45

Try making the solid timescale 100x larger and as a second test the same as the fluid time scale.

mactech001 January 27, 2010 02:12

1 Attachment(s)
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......

ghorrocks January 27, 2010 16:49

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?

stumpy January 28, 2010 15:45

Turn on double-precision too.

mactech001 January 29, 2010 00:58

1 Attachment(s)
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.

stumpy January 29, 2010 17:47

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.

ghorrocks January 30, 2010 06:45

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?

mactech001 February 2, 2010 23:31

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?

ghorrocks February 3, 2010 04:58

In V11 you need to select double precision in solver manager or the command line. In V12 you can select it in CFX-Pre.

All times are GMT -4. The time now is 03:55.