[jackzhushen]

Hi guys:

I was doing a compressor stage (NASA Stage 35) computation with CFX.

At first I used Average Static Pressure outlet and computations converged.

Then I changed the outlet condition to Mass Flow Rate for computations at lower mass flow condition.
Computations diverged and showed: "Fatal Overflow in Linear Solver"

After that I did several changes, including:

• defining run w/o initial values (last converged case with pressure outlet),
• changing the mass flow rate from low to high,
• changing the turbulence model from SST to k-w or k-e,
• changing another mesh.

However, no one converged.

But the strange thing is, I tested some other compressors with mass flow outlet, including high speed and low speed compressors stage. All these computations converged.

So what might be the problem? Mesh quality, initial solution, or computation domain?

Thanks!

[ghorrocks]

If your inlet is a mass flow boundary (or a related type, such as velocity) then having a mass flow boundary on the outlet will always crash as the simulation is ill-posed.

That is why the recommendation for boundary conditions where you have one inlet and one outlet is for one of inlet or outlet to be a mass flow and the other to be a pressure boundary.

[jackzhushen]

Thanks for your reply!
But a total pressure and total temperature condition was imposed at inlet.
So I suppose it's not the problem of inlet condition.

[ghorrocks]

OK, if you don't have mass flow boundaries for both inlet and outlet it is caused by something else.

Have a read of the CFX Modelling guide as it has useful recommendations on boundary condition selection.

And in your case you will need to make sure the flow rate you are specifying is physically possible - for instance higher than the choked flow for a duct.

And if that is not the cause consider the normal things to look at for increasing numerical stability, described here: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[jackzhushen]

Many thanks for your detailed guidance!

I think I've got this problem fixed to some degree.

At "Boundary Details" tab, I checked the "Mass Flow Outlet Constraint" box after setting a "Mass Flow Rate" outlet, and selected "Pressure Shape Constrained", filling in the "Pres. Profile Shape" with a roughly matching pressure value.

Then cases with mass flow outlet converged, however, with less good stability.

Cases at higher mass flow conditions converged better, while the inlet mass flow monitoring curve oscillated with really large amplitude at lower mass flow rate.

I supposed the "Pressure Shape Constrained" option might provide a more robust boundary condition, initial guess or something else for this case.

I have not validated the results from this outlet condition yet. More works to be done.

If you have some ideas about this circumstance, I'm looking forward to your words.

[a.nagib]

Hi Zhu,

you can use the prescribing radial equilibrium with a specified hub (or casing) static pressure, the equation is in http://www.grc.nasa.gov/WWW/5810/rvc...ima-cstall.pdf in page 6.

I am currently facing the same problem that you had I am simulating NASA Stage 35 with Inlet total P &T B.C. and mass flow rate @ the outlet with no conversion, I tried using pressure specified opening boundary after adding the flowpath inlet domain before the rotor and outlet domain after stator and waiting for the results.

After that I will use the equation mentioned above and mass flow rate constrain that you mentioned.

could you please tell me what value did you chose for the average static pressure and from where did you get it?