ANSYS CFX Solver Domain Imbalance
 

I am doing CFD analysis of pelton turbine using ANSYS. THe CFX solver shows domain imbalance, attached. My domain consists of a stationary domain and rotary domain. I was looking if anybody could explain the physical meaning of domain imbalance. The value changes from positive value to negative value.

The domain imbalance is simply the sum of that variable over the domain's boundaries. So for mass, it is the the sum of all the inlets plus the outlets (noting that flow into the domain is positive and out is negative). If conservation is achieved this will sum to zero (assuming no mass sources or sinks, or accumulation of mass in the domain). If it does not sum to zero the imbalance gives you the magnitude of the imbalance and it is up to up to determine if that is a problem or not. This is also done for momentum, heat and any other equations you are using.

The imbalances you are showing are pretty large for most applications so most people would not consider your simulation converged. So best run it longer to reduce the imbalances. Even better, add imbalances to the convergence criteria and it will keep running until the imbalances are down to your defined tolerance.

In solver control, select "Consvervation Target" and set it to a small value, say 0.01 or anything of your choice (between 1 and 0).

Thanks for your hint to judge the conservation yourself. But what do you think on this one:

I have a rotating Domain (x-axis), with a cylindrical opening. My residuals and monitor points seem to converge pretty nicely, but the imbalances seem really high. U-Mom is quite low with 1% imbalance whereas W-Mom and V-Mom are between 9% and 11%.
I would suspect this to be due to the rotation of the opening and the air in and outflow.

Cheers,
Marcel

Possibly. But it does mean that it is highly likely your simulation is not adequately converged. You might be able to fix it by simply running the simulation longer (I presume this is a steady state or frozen rotor simulation).

Thank you for your advice. yes it is steady state, but I already run about 300 iterations with auto timestep. don't really know if thats adequate as I'm not too long in the cfd business.

Then simply run it longer and watch the imbalances in the solver manager. They should by converging to zero - if so then just run it longer for tighter convergence. If they are still bouncing around consult this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thank you, I will try that.

So far I used the Imbalances a good indicator for my convergence.
What I encountered now is hard for me to grasp. The p-Mass-Flow is fluctuating between 100% and -100%, jumping like square function.
Hence I was asking myself how it is calculated exactly. Since my userpoints indicate good convergence, I didn't think this behaviour shows bad convergence.

That is why imbalances are not the default convergence option.

Image this: If you have a box with only a single opening, mass conservation tells you that there will be no net mass flow through the opening. But in a numerical simulation there is errors and noise, so there will be a tiny flow caused by numerical noise (let's call the flow rate m). The imbalance calculation is the imbalance divided by the total flow, so that is m/m which is either +1 or -1 depending on the flow direction. And that is why the imbalances flick between 100% and -100%.