Hello, does anbody know, where can I see, which equation does not fulfill the conservation target in my simulation???Is it possible to see it from the out file where linear solution is shown? (Without conservation taget checked 2 or 3 coefficient loops are used, but in case when I choose conservation target (even it does not matter is it 0.01 or 0.9 ) then the maximum number of coeff. loops always remain with the best wishes Target

http://www.cfd-online.com/Wiki/Ansys...ible_answer.3F

I will try once again, may be somebody could help me to solve the problem...

The problem is that my transient heat transfer/CFD simulation does not satisfy the "conservation target". That I know because the solver goes through the maximal number of coeff. loops (set 10 or 20)even then when I set conservation target to maximal possible 0.99. In this simulation timestep is small enough, in case of not asking conservation target to be satisfied,- convergence of Max and rms residuals is very fast.

It would be important for me to know, which equation exactly does not satisfy the conservation target. It could give me an answer why good convergent (when looking on rms or max residuals solution is not fully reliable).

Post a copy of your command file.

Hi, it is various pages... I am speaking about that part in definition exactly.

SOLVER CONTROL:

ADVECTION SCHEME:

Option = High Resolution

END

CONVERGENCE CONTROL:

Maximum Number of Coefficient Loops = 8

Timescale Control = Coefficient Loops

END

CONVERGENCE CRITERIA:

Conservation Target = 0.99

Residual Target = 1e-06

Residual Type = MAX

END

TRANSIENT SCHEME:

Option = Second Order Backward Euler

Timestep Initialisation Option = Previous Timestep

Make the following changes:

CONVERGENCE CONTROL:

Maximum Number of Coefficient Loops = 8 -> Change to 3 to 5

Timescale Control = Coefficient Loops

END

CONVERGENCE CRITERIA:

Conservation Target = 0.99 <- Remove this entirely. This was the cause of your problem. Understand what it does before trying to use it again.

Residual Target = 1e-06 <- Set too low, change to (1e-5 - 1e-4)

Residual Type = MAX <- RMS may be more appropriate for your application depending on your mesh quality.

END

You can monitor equation imbalances in the solver manager... make a new monitor and look at the 'Imbalance' fields.

You can also add the expert parameter 'monitor totals=t' to get the data dumped to your out file every timestep.

Thank you Joe for suggestion. I know that it is working without conservation target and with rms is converging very well. Unfortunately solution becomes not physical - not stable and that is why I wanted to keep balances in each inner loop and started to experiment with changing the value of conservation target - 0.01 did not work so I tried larger numbers and none of it worked (solver reached the number of maximal coeff. loop and continued the next timestep).

Yes, that is exactly what I am interested in - to understand the role of conservation target to find, which equation does not allow to satisfy the balances inside each inner loop of transient simulation.

Thank you Phil!!! I plotted equation imbalances! I can see that problem is with P-mas imbalance - after some iterations it is just equal to 1.

I have a fixed amount of fluid without inlet or outlet but I calculate transport equation for virtual additional variable inside it to simulate some other processes. Could P-mas imbalance =1 because of that or I have to look for some other problem?

If your solution is becoming unphysical it is much more likely that something else is causing the problem, rather than just poor equation imbalances.

I call unphysical the situation when the solution, which is expected to be axisymmetrical becomes non-axisymmetrical. In some cases it remains symmetric, in some not - that is why I wanted to look more careful on balances...

Is there a possibility to apply conservation target to each equation separately (not to apply for one equation)?

Yes, I think that is the problem. I am quite sure you can define conservation targets of each equation. Either in Pre, otherwise in the command editor.

Another suggestion is to use double precision. This might help when you want to achieve deep convergence with large and small numbers..........

Astird

My guess is that P-mass equation imbalance =1 is because of density temperature dependence, included in the model.

My present question is - does anybody knows how is it possible to set conservation target for each equation seperately?