Hey Guys,

I have a new problem. I have done a "easy" manifold.

Now the solver told me that the flow reverses. Has anybody an idea?

I'm using StarCAT5 3.02.005 with StarCCM 3.02.003.

Regards, Martin

martin

it means that you have an inflow at either an outlet or pressure boundary. Do you have your 'outlet' far enough away from your manifold geometry.

allan

Hello,

I make my boundary's with CATIA, I think the position should be okay. I have a stagnation inlet (1.0 psi) and 4 pressure outlets (each 0.903 psi).

I think I have a problem in my mesh.

Regards, Martin

Hello,

May be you should work with field function at pressure outlets

Rabat

Can you explain me what this mean?

I had talked to a friend, he had add to my SIM a velocity speed in the air and his moddified SIM works in my Star CCM. When I make the same under StarCAT it don't work. I have tried a bigger pressure difference. Inlet 14.7 psi, outlet each 13psi. Air start pressure 14.7 psi and the speed in one direction.

I'm not a expert in Star, I'm on the beginning but I think this seems to be a very easy problem and it don't work.

Hello,

I looked in the manual for this problem. "In STAR-CCM+, pressure outlet boundaries are designed to permit recirculation, although a unique solution may not exist resulting in convergence problems.

* Recirculation will cause a non-uniform static pressure at the boundary.

* If a uniform static pressure is desired, the mesh should be rebuilt with the outlet region extended in such a way as to prevent recirculation.

* Convergence problems due to unsteady recirculation will be indicated by the number of faces at which reversed flow occurs changing from one iteration to the next. (The number of faces is printed in the warning messages in the output window.) If this occurs, the outlet region extended in such a way as to prevent recirculation."

Does I understand this write? I had made the 4 outlets longer. The error at the beginning I don't have now. Only the inlet is reversing now. Ok I thought make it longer, but this didn't helps. During the Solve the flow reverse very often. Pressure I set to 1,1Bar on inlet and air, 1.0 Bar on the 4 outlets.

Any ideas?




Thanks Martin!

Martin

I don't think you should use a stagnation inlet, that's for high mach number flows.

Change your pressure inlet to mass flow inlet and set a sensible mass flow. Run this for 100 or so iterations then change it to a pressure outlet and set your pressure.

If you are assuming the flow is incompressible then I suppose you could use a velocity inlet instead

allan

Hmm this idea is good. I will try it. I want the mass flow of each outlet to see what outlet get's more or less mass flow. I thought on a stagnation inlet because I had worked on a flow bench. I will tell you if it works. Thanks for all!

Martin

another thing, models with only pressure boundaries are more difficult to solve. You may need to tighten up the relaxation.

A stagnation inlet may be ok, I'm more into star-cd than ccm+, but I've run models sucessfully with just pressure outlets. Then only problem with this is that it will tell you that you have reverse flow at the outlet where the flow is inwards

allan

Hey allan,

I think the "solver" should be the same on both. When the settings are wrong in both cases the problem is inconsistent. I will try it, but I think after changing the boundary StarCAT will make a new mesh and a new solve run from beginning. But I will try.

Thanks!

Regards, Martin

Hey allan,

I tried it. It seems to work. But I don't understand why the flow only goes in the middle outlets... I will try some other pressures, maybe difference is too high (13psi and 14.7psi) or start air mass is too high (0.05kg/s).



Regards, Martin

Martin

Are you solving this ideal gas law i.e. compressible flow? If not try that. Also with mass flow inlets, set the relaxation to about 0.2 on pressure, 0.5 on velocity, temperature and turbulence. Run for a bit, 100 odd iterations, maybe a bit more. Change to pressure outlets, keep the same relaxation. Run until the residuals are quite low. Stop and save. Set the relaxation factors back to thier default and continue running.

I think what you have here is a valid solution, just not the one you want. I have had problems with this on a similar type of flow model.

cheers

allan

[Maddin]

Hey Allan,

New Forum here, nice.
I normally use "constant density". When I change it to "ideal gas law" here makes me some more errors...

Calculating grid flux in region Volume Mesh:subdomain-1
Initialization of SegregatedFlowModel requires an additional pass...
Initialization of SegregatedFlowSolver requires an additional pass...
**
** Warning: Initializing turbulent flow using intensity and zero velocity in subdomain-1!
**          Velocity magnitude of 1 m/s assumed for initialization.
**
**
** Warning: Initializing turbulent flow with density unavailable in subdomain-1!
**          Density of 1 kg/m^3 assumed for computing initial turbulence quantities.
**
Warning: Wall distance limited to 1e-006 in 7 cells in region subdomain-1
Temperature corrections limited in 3551 cells in region subdomain-1
max. Temperature limited to 5000 in 297 cells in region subdomain-1
Turbulent viscosity limited in 4914 cells in region subdomain-1
 Iteration     Continuity     X-momentum     Y-momentum     Z-momentum         Energy            Tke            Tdr
         1
   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00
pressure corrections limited in 56629 cells in region subdomain-1
Temperature corrections limited in 2434 cells in region subdomain-1
max. Temperature limited to 5000 in 87 cells in region subdomain-1
Turbulent viscosity limited in 24 cells in region subdomain-1
         2   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00
         3   9.029993E-01   1.000000E+00   1.000000E+00   1.000000E+00   1.000000E+00   4.318042E-01   1.000000E+00
pressure corrections limited in 56619 cells in region subdomain-1
Temperature corrections limited in 3341 cells in region subdomain-1
max. Temperature limited to 5000 in 47 cells in region subdomain-1
Turbulent viscosity limited in 133 cells in region subdomain-1
pressure corrections limited in 56617 cells in region subdomain-1

This is a run with ideal gas law.

Mass flow I set to 0.05kg/s. Pressure to 1.0bar at the outlets and 1.1bar the air.
I will try bigger flows. I don't understand why it's seems to be very difficult to make a correct run.
I send a friend the CCM File whit my problem.
He told me that he only adds a direction of the flow in the start settings (80m/s) and it works.
When I get the file back it works.
When I tried to make the same settings in my file (which I send him before) it don't works.

Regards, Martin

[Maddin]

Ok... I tried very simple body's to "solve" the problem.
First with 2 outlets, then 3 and the last with 4 outlets.
The first picture I had made a 100step run.
Inlet velocity 4m/s
Outlet velocity -2m/s
On the later body's I used 8m/s to get -2m/s. I think you see it.
The second picture of the body is the change boundarys to pressure. On the inlet 1.1bar, on the outlet 1bar.
Problem for me, the mass flow don't changed.
Why? Velocity to high/too low in the first calculation?

[Maddin]

Sorry for the multi post but I can only put 10 pictures in one post.

I have seen this, what will Star tell me with that? Somebody an idea?
Did this just happens and it's no problem?





I did a run with mass flow inlet (0.2kg/s) and pressure outlets (100.000Pa because change it to bar on every change is too much time for me ) and run 100 steps. Then I changed the mass flow inlet to pressure outlet with 120.000Pa.
The massflow through this boundary don't changed but the massflow on the other changed more.
The middle neraly the same (0.0501-0.0502Kg/s). The first outlet the smallest mass mass flow (0.043Kg/s) and the last biggest mass flow (0.056Kg/s).
This seems to be right because I know this effect on manifold.
I'm on the right track? What do you think?