<U>Problem:</U>

I am doing a CHT simulation of the cooling system of a pump. My model consists of a Motor covering (whose inner wall is the source of heat), outer Outer covering and inbetween them is the fluid. The fluid is cooled in a flange. I am simulating this full setup with flange.

In order to finalise with the boudary layer, I am doing a simulation only with the fluid region, which travels from the flange to the region between Motor covering and Outer covering. The fluid domain has 3.3 M hexa cells. I am doing with a SST turbulence and gamma model 260 transitional turbulence. The model has a Inlet with mass flow rate and opening with open pres. and dirn and both inlet and opening with a fixed temperature. I had set up a Conservation target of 0.01 and Max residual target of 1e-5

I did the simulation with a autotimescale (0.1s) and after about 100 iterations the Momentum, Mass and Heat transfer residual graphs keeps oscillating. I re-tried the simulation with a physical timescale of 0.4s and I found no improvement. For both the simulations I did until 500 iterations.

<U>Results:</U>

The max. RMS residual is 1.2e-04

My domain imbalances are:
Domain 1 Domain 2
U-Mom 0.0642 % -0.0879 %
V-Mom 0.0258 % -0.0103 %
W-Mom 0.0266 % -0.0162 %
P-Mass 0.0659 % -0.0667 %
H-Energy 0.0721 % -0.0661 %

The monitor points of Temperature on both the domains are stable (horizontal graph).
The monitor point of Velocity on Domain 2 is stable and the one in Domain 1 is not.

<U>Questions:</U>

1. Has my simulation converged?
2. What does the wavy nature of the residuals imply?
3. What does the monitor point velocity on domain 1 imply while the velocity on domain 2 is stable?


Any sort of help is really appreciated.
Regards,
Subha.

Is this perhaps indicating that the real solution is oscillatory not steady (e.g. something like vortex shedding, intermittant plumes, etc would occur in reality...)? That's certianly what I happened in a recent calculation of mine.

So, if you can rule out a localised mesh problem, etc, then perhaps you need to consider a time-dependent simulation to see if you can capture any oscillatory behaviour explicitly? Of course that's time consuming, so don't just trust me: I think the ANSYS documents give advice on this, and it's covered in the best practice guidelines and FAQs linked from this website - I saw it somewhere again just yesterday and will post the exact link if I find it - so investigate the advice there first!

Anyway, good luck, andy

Hi Subha,

It may help to view the regions where the residuals are still large. You may have an isolated region where the solution is changing but is having little effect on the rest of the solution domain. To view the residuals you can either enable the expert parameter "output eq residuals = t" or enable the output of residuals in Pre from the Output Control panel.

Visualizing the flow in the non-converged region may help determine the issue. It could be physical, due to a separation for instance, you numerical, due to poor quality elements or large expansion ratios (a very common problem arises where you have a very fine inflation layer and a massive jump in volume from the last prism to the first tet).

I would also try varying the timestep a bit further. You can try running with a very large timestep (say 40 [s] or a very small one (.04 [s]). You should also compare the timestep with the actual advection time. To do so, calculate streamlines from your inlet and look at the maximum time on the streamlines as well as the average time on the streamlines (which eliminates the effects of a few streamlines getting hung up in separated regions). The average time on a streamline actually serves quite well as an estimate of the necessary physical timescale.

-CycLone

http://www.cfd-online.com/Wiki/Ansys...gence_criteria