[CFD_SG_01]

Dear OpenFOAMers,

As an OpenFOAM newbie I do solicit your help for an OpenFOAM case setting.
I work on OpenFOAMv2312 (OpenFOAM.com) and try to set a centrifugal pump case from a polymesh generated from StarCCM+.

Here is the setting based on the tutorial Mixer2D.

Solver: pimpleFOAM
Mesh: 3 regions (Inlet, impeller and volute)
Turbulence: Laminar (no turbulence for the moment only momentum and pressure)

• U
  //Inlet
  Stator_1_FlowdomainInflow
  {
  type flowRateInletVelocity;
  volumetricFlowRate constant 0.001;
  }
  
  //Outlet
  Volute_1_FlowdomainOutflow
  {
  type pressureInletOutletVelocity;
  value uniform (1 0 0);
  }
  //Inlet
  Stator_1_FlowdomainInflow
  {
  
  type zeroGradient;
  }
  //Walls
  "(Impeller_1_FlowdomainShroud|Impeller_1_Flowdomai nBladeSS|Impeller_1_FlowdomainBladeLE|Impeller_1_F lowdomainBladePS|Impeller_1_FlowdomainBladeTE|Impe ller_1_FlowdomainHub|Impeller_1_FlowdomainCasingHu b|Stator_1_FlowdomainShroud|Volute_1_FlowdomainCut Water|Volute_1_FlowdomainDiffuser|Volute_1_Flowdom ainSpiral)"
  
  {
  type noSlip;
  }
  
  //AMI Interface
  "(AMI1|AMI2|AMI3|AMI4)"
  {
  type cyclicAMI;
  }
  
  

• P
  
  //Inlet
  Stator_1_FlowdomainInflow
  {
  
  type zeroGradient;
  }
  
  //Outlet
  Volute_1_FlowdomainOutflow
  {
  type fixedValue;
  value uniform 101.629889;
  }
  
  
  //Walls
  "(Impeller_1_FlowdomainShroud|Impeller_1_Flowdomai nBladeSS|Impeller_1_FlowdomainBladeLE|Impeller_1_F lowdomainBladePS|Impeller_1_FlowdomainBladeTE|Impe ller_1_FlowdomainHub|Impeller_1_FlowdomainCasingHu b|Stator_1_FlowdomainShroud|Volute_1_FlowdomainCut Water|Volute_1_FlowdomainDiffuser|Volute_1_Flowdom ainSpiral)"
  
  {
  type zeroGradient;
  }
  
  
  
  //AMI Interface
  "(AMI1|AMI2|AMI3|AMI4)"
  {
  type cyclicAMI;
  }
  }

N.B. A scotch method is applied to use decomposePar

//- Force AMI to be on single processor. Can cause imbalance with some
// decomposers.
//singleProcessorFaceSets ((AMI -1));

numberOfSubdomains 8;

method scotch;

coeffs
{
n (2 2 2);
}

Here are the issues:
It automatically diverges. Courant number value quickly "explodes".U and P iterates more than 1000 times.

It seems the AMI interfaces work well and the rotation too. But I still do not understand why it diverges.
If I set runTimeModifiable as true and adjustTimeStep as yes it iterates to keep the courant number under 5 (the value I set) but the deltaT quickly decreases down to 1e-11 s.

Is there any subtlety I miss to perform the computation case?
Do you know how to increase iteration with a minimum of 5 per time step?

Thank you in advance for your help

[CFD_SG_01]

Hello,

I keep moving forward on this case and I've finally found what the was the initial problem. The issue came from the mesh. It seems like openFOAM solver is not as robust as StarCCM+ solver. There were few cells with a wrong aspect ratio.

I keep trying to work on the case and today I find some very high velocity values close to the impeller/volute AMI face zone. Is there any subtlety to set to avoid such numerical aberration?

Thank you in advance for your help

[CFD_SG_01]

Hello,

Here are the latest news regarding the case I try to set.

The case seems to work weel when I use simpleFoam solver combine with the MRF method but it is still extremely difficult to compute it using pimpleFoam with slidingMesh method.
The courant number explodes as well as the maximum U magnitude value
(see below the terminal extraction)

fieldMinMax fieldMinMax write:
min(mag(U)) = 0 in cell 0 at location (0.004675068 -0.006483044 -0.04850577) on processor 0
max(mag(U)) = 2.445269e+21 in cell 202371 at location (-0.0001384865 0.007978789 -0.001543877) on processor 0
min(k) = 0.0037199 in cell 65822 at location (-0.005791429 -0.005494721 -0.0945) on processor 0
max(k) = 0.375 in cell 66247 at location (0.1141571 0.03605855 0.008828515) on processor 1
min(omega) = 20 in cell 65822 at location (-0.005791429 -0.005494721 -0.0945) on processor 0
max(omega) = 6.292383e+10 in cell 198227 at location (0.02441025 -0.005510982 0.00279894) on processor 6
min(p) = -1.737645e+30 in cell 320636 at location (-0.02849686 0.01301534 0.006458972) on processor 0
max(p) = 101.6299 in cell 65160 at location (0.115 0.02611258 -0.002615524) on processor 1
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Courant Number mean: 4.184367e+11 max: 2.293194e+14
deltaT = 8.735595e-24
Time = 0.000104053

Does anyone have ever experimented such issue ?
Thank you in advance for your help

[Yann]

Hello,

Have you checked where you get these high velocities? Is it still in the vicinity of the AMI interfaces?

You may have a look to you log file and check what you get on AMI:

AMI: Creating AMI for source:AMI1 and target:AMI2
AMI: Patch source faces: 96
AMI: Patch target faces: 96
AMI: distributed
AMI: Patch source sum(weights) min:1.00007 max:1.00007 average:1.00007
AMI: Patch target sum(weights) min:1.00007 max:1.00007 average:1.00007

The weights should be close to 1. If you have min/max values far away from 1 it might indicates something is going wrong with the AMI.

You can try using the moveDynamicMesh utility. This will allow to move the mesh without solving the flow. It can be useful to check if your mesh is moving as expected and if there is no issue at the interface (such as deformed or overlapping cells during the mesh motion due to wrong AMI definition)
There is also a -checkAMI option with this utility to write VTK files of the interfaces with the corresponding weights. If there is something wrong with the AMI it can also be helpful to see where the problem lies.

Regards,
Yann