Dear all,

the message listed below is well known, the point that I do not undestand is why by starting already solved *.cfx file (by which I did not receive any error messages)and now I am changing only the mass flow rate at the inlet and by the solver I received it from iteration 20.Does someone of you have any ideas?Thanks in advance

--------------------- A wall has been placed at portion(s) of an OUTLET boundary condition (at 0.6% of the faces, 0.7% of the area) | to prevent fluid from flowing into the domain. The boundary condition name is: outlet. The fluid name is: Water. If this situation persists, consider switching to an Opening type boundary conditi

IMHO, most likely, that is because you changed the mass flow rate, then the flow generates ciurculation cross outlet boundary.

This is not surprising, as you changes the inlet BC. CFX may calculate some backflow at your outlet for smaller mass flow. I do get similar problem when I reduce the inlet flow velocity. Just change your outlet BC to opening and see if it helps.

Now I tried by setting inlet: static pressure and outlet: mass flow rate, but it does not help. I'll try with opening as well, though I suspect that this will influence the correct result of my model, because I am modelling one half of a tube with coil inside. Do you know how an "opening" behave when there are symmetry BCs? Thanks again

Also, Anna

It may not be a problem if it only places a wall at 0.0x% depending upon where your area of interest is. If it is at the outlet, and the mass flow is at the required value, then the wall at the inlet may have no bearing upon the results at the outlet.

However, you must be 100% certain that this is the case before you can 'ignore' the wall at the inlet.

Adam

Hi Adam,

I set inlet: static temperature and mass flow

outlet: pressure

If I put now an opening do I have to keep the same inlet conditions? What do you think? Thanks a lot

I'd stay clear of using an opening for your outlet, as they are inherently unstable and I suspect will introduce more errors in the simulation.

I don't know by what amount you changed your mass flow from the first run, but if it is a considerable amount (relatively) then that may be the issue. Try a smaller mass flow change.

Also, if it is still a problem, then you may want to ask yourself if you are using the correct geometric approximation to the problem and if you are using the correct turbulence model.

Adam

yes Adam, you are right. Now my flow rate is 0.4 kg/s, I would like to reduce it to 0.1kg/s and the hydraulic diameter is 0.1m. So maybe in this case the SST turbulence model is not an appropriate one.

Anna,

I would reduce the mass flow to 0.25 before going to 0.1.

I suspect that may be the problem, as you are in effect reducing the mass flow to only a 1/4 of the orginal mass flow.

As for the SST, if the flow is definetley turbulent, then I would use the SST model as it is far superior to the ke model, especially if you have a y+<10

Adam

I'm a bit confused now. It's always good to describe your problem before asking a question or give a http link if you did it before.

When you get this message again, stop the solver and you should get the result where the inflow at outlet has occurred. Plot the velocity in Post to compare the difference between your new and old solutions. Check if the backflow region at the outlet is physical or not.

I'll have doubt if this message will disappear when you try SST model. Standard ke is far more stable than SST model.

Instead, you should also reexamine if the outlet boundary condition remains valid when you reduces the inlet mass flow.

I would disagree, especially in separated or recirculating flows, as the ke model does not predict separation very well at all which can lead to incorrect results.

It all depends upon your geometry and your flow conditions.

I didn't mean that ke solution is correct. If you get message like this in ke model, you will most likely get the same message using SST model. Switching turbulence models doesn't help in solving this problem, but it's no harm to experiment and check it out yourself anyway.

Besides, I'll not jump into conclusion too fast that SST is defintely going to work better than ke. Many publications also show that the more advanced turbulence model like RSM doesn't help improving the accuracy at all. In logic, RSM should work better than two equation model, as RSM includes more physics in the model.