[Simplyyy]

I am running a double-pipe counter flow heat exchanger on CFX. The heat exchanger is suppose to run on Supercritical CO2, therefore I generated a Real Gas Properties (RGP) file using the generator tool for S-CO2, but whenever I run it on the solver, I keep getting this warning after each iteration in the solver:

****** Warning ****** |
| |
| Independent variables were clipped during table generation |
| at: END OF TIME STEP |
| 0 detailed warnings were printed because the maximum |
| number of warning messages was exceeded. |
| |
| The maximum number of detailed table clip warning messages can be |
| controlled with the following expert parameter: |
| |
| max table messages (default: 0) |
| |
| Please increase the number, if you need further details of the |
| locations and variables involved.


Though the solution does converge. I re-created the RGP file changing the pressure range to include the atmospheric pressure (Default reference pressure in CFX) and I noticed that the warning stops appearing! But I do not understand why does this happen since the atmospheric pressure is just a reference.

If anyone experienced similar issue please share

I am using ANSYS 15

[awesim]

Hello Simplyyy,

I got the same message once. I was simulating air with humidity and hence defined a user material.

The message, that variables were clipped during table generation, indicates that the range set by the user for generating the table for temperature and pressure is too small.
So it could be that at one point during your simulation you reach a pressure that lies outside the specified interval. By decreasing the lower bound of your table you can prevent that. Probably that is what you have done by setting it to atmospheric pressure.

Another advice: If you use user functions to model material properties (such as conductivity or heat capacity in terms of temperature) try to create enough sampling points since CFX only interpolates linear between them. You could incur a large error through this.

Hope this helps,

Simon

[Sumanth_094]

[QUOTE=awesim;529057]Hello Simplyyy,


Another advice: If you use user functions to model material properties (such as conductivity or heat capacity in terms of temperature) try to create enough sampling points since CFX only interpolates linear between them. You could incur a large error through this.


Could anyone ellaborate on the last part about the sampling points?
I have an expression evaluating the C_p using Temperatures and I am using a User defined turbulent heat flux closure. I end up encountering the table bound error which somewhat messes up the simulation. The solver stops and doesn't really say what the exact error was.

Any help would be much apppreciated.
Thanks a lot.

[Opaque]

If the case produces meaningful results w/o the user-defined turbulent flux closure, there is nothing wrong nor out of bound errors, correct?

Once a non-standard modification of the turbulent flux closure is introduced, and the software misbehaves, it is a sign the modification is not consistent with the other pieces of the model; consequently, the source of the problem. Then, the next step to understand is where the inconsistency is coming from.

During non-linear iterations, the software may understandably get outside of the provided range for properties, and once those properties are clipped or else w/o respecting thermodynamic principles all kind out of bound errors will show up.

Hope the above helps,

[Sumanth_094]

Yes, that makes a lot of sense. I figured that using too many complexities in the model just increases the probability of the model diverging, especially when using User defined models. So, I am reducing them one by one to figure out what could have lead to the problem but at the same time I am running out of time. :/

One thing I also wanted light to be shed on is that, I am starting this simulation with a result file as initialization and since the result file had converged pretty well, the new simulation starts off with lower imbalances and RSM residuals and they stay in the same orders for 20 odd iterations before the whole clipping problem starts.

Usually, one uses a initial file as guess (in best case scenario, the result file being almost identical to the current simulation being performed) so as to run lesser iterations and get convergence faster.

The question here really is whether there exists like a rule of thumb which says one has to run these many minimum iterations although its being very well initialized?
My simulation results are pretty good with imbalances less than a percent and RMS values in the order of 10^-5 and below till 20 odd iterations. Can I say the simulation has converged and hence stop before it blows up in my face?

The thing sounds to me like cheating but I am really not that experienced yet to make a call on this. Do fill in with your valuable inputs.
Thanks you in advance