[Stanislav_K]

Hello for everyone,


I want to perform CFD analysis of centrifugal pump to find the performance of pump. I have the tested data for this pump.


Definition of the BCs (see Figure 1):

Internal Volume Flow Rate on INLET

Environment Pressure on OUTLET

Real wall (Stator) - marked as blue in the Figure 1

Local Rotating (Averaging) Region – 2950 RPM. Rotating region is defined by the outer shape of the impeller (marked as green*in the Figure 1)


Surface Goals:

Mass Flow Rate Inlet

Mass Flow Rate Outlet

Av. Static Pressure Inlet

Bulk Av Static Pressure Outlet (at the point of the discharge flange)

Torque on impeller


Equation Goals:

Pressure Drop* { Av Static Pressure Outlet}-{Av Static Pressure Inlet}

Efficiency {Pressure Drop}*{Inlet Volume Flow 1:Volume flow rate:5.000e-003}/{Rotating Region 1:Angular velocity:3.089e+002}/{SG Torque on Impeller}



Most of the time I got an error "Solver Abnormally terminated" after going circa 300 iterations.

If it got solved, I observed that Mass Flow Rate at inlet and outlet were not equal.

They had a huge difference in value.

The pressure difference and torque value were also very high (Figure 2.).


Kindly suggest and help me out what changes I should make in the set up to achieve the required results.


Thanks in advance.


Stan K.

[the_phew]

I've been running a lot of centrifugal blowers in Flow Sim lately. Some things I've learned:
1.It's VERY sensitive about the clearances around the rotating region. It doesn't like the RR to be coincident with walls, with preferably several cells of clearance between the RR and any solids. If you need to model a very small clearance, you either need a ridiculously fine mesh or just let an axisymmetric portion of the casing/volute/whatever rotate with the RR (not strictly correct, but at least it lets you run a simulation). Otherwise, you can just artificially increase the clearances until it will run
2.It's sensitive about inlet mass/volume flow boundary conditions. I usually initialize it with a total pressure inlet BC, then iterate the inlet P0 manually until I get the correct mass/volume flow. Once you are in the ballpark, you can usually restart with a volume flow BC, however. But it really struggles with the startup transient with centrifugal turbomachines combined with mass/volume flow BCs.

The issues with #1 usually cause the solver the terminate before the first iteration, so that may not be your main concern. But try running with a total pressure inlet BC and see if it converges.

For any turbomachine, looking at relative streamlines in the rotating reference frame will tell you a lot about what's going on in your simulation. Unfortunately, Flow Sim doesn't let you monitor these during a run, so you have to save the results and inspect periodically. If the blade incidence is really high or low, you probably aren't near the design condition for that rotor.

[mariconeagles96]

Originally Posted by Stanislav_K

Hello for everyone,


I want to perform CFD analysis of centrifugal pump to find the performance of pump. I have the tested data for this pump.


Definition of the BCs (see Figure 1):

Internal Volume Flow Rate on INLET

Environment Pressure on OUTLET

Real wall (Stator) - marked as blue in the Figure 1

Local Rotating (Averaging) Region – 2950 RPM. Rotating region is defined by the outer shape of the impeller (marked as green*in the Figure 1)


Surface Goals:

Mass Flow Rate Inlet

Mass Flow Rate Outlet

Av. Static Pressure Inlet

Bulk Av Static Pressure Outlet (at the point of the discharge flange)

Torque on impeller


Equation Goals:

Pressure Drop* { Av Static Pressure Outlet}-{Av Static Pressure Inlet}

Efficiency {Pressure Drop}*{Inlet Volume Flow 1:Volume flow rate:5.000e-003}/{Rotating Region 1:Angular velocity:3.089e+002}/{SG Torque on Impeller}



Most of the time I got an error "Solver Abnormally terminated" after going circa 300 iterations.

If it got solved, I observed that Mass Flow Rate at inlet and outlet were not equal.

They had a huge difference in value.

The pressure difference and torque value were also very high (Figure 2.).


Kindly suggest and help me out what changes I should make in the set up to achieve the required results.


Thanks in advance.


Stan K.

Hi! Any workaround on this? I am also trying to model a similar problem and yes solver stopped. And when i got to run it and adjusted the domain and lids, same problem with mass balance not being equal.

[mariconeagles96]

Originally Posted by the_phew

I've been running a lot of centrifugal blowers in Flow Sim lately. Some things I've learned:
1.It's VERY sensitive about the clearances around the rotating region. It doesn't like the RR to be coincident with walls, with preferably several cells of clearance between the RR and any solids. If you need to model a very small clearance, you either need a ridiculously fine mesh or just let an axisymmetric portion of the casing/volute/whatever rotate with the RR (not strictly correct, but at least it lets you run a simulation). Otherwise, you can just artificially increase the clearances until it will run
2.It's sensitive about inlet mass/volume flow boundary conditions. I usually initialize it with a total pressure inlet BC, then iterate the inlet P0 manually until I get the correct mass/volume flow. Once you are in the ballpark, you can usually restart with a volume flow BC, however. But it really struggles with the startup transient with centrifugal turbomachines combined with mass/volume flow BCs.

The issues with #1 usually cause the solver the terminate before the first iteration, so that may not be your main concern. But try running with a total pressure inlet BC and see if it converges.

For any turbomachine, looking at relative streamlines in the rotating reference frame will tell you a lot about what's going on in your simulation. Unfortunately, Flow Sim doesn't let you monitor these during a run, so you have to save the results and inspect periodically. If the blade incidence is really high or low, you probably aren't near the design condition for that rotor.

Hi! Mine is solver terminated after the 1st run. It says "The inlet boundary condition may conflict with the supersonic flow regions Flow opening BC: Inlet". Can you help me out? Thanks!

[the_phew]

Originally Posted by mariconeagles96

Hi! Mine is solver terminated after the 1st run. It says "The inlet boundary condition may conflict with the supersonic flow regions Flow opening BC: Inlet". Can you help me out? Thanks!

For most internal flows, you should use a total pressure inlet BC, and vary static pressure on the exit BC to achieve your desired flow rate (this is true in every CFD solver). Once you get through the startup transient, you can probably switch to a volumetric flow rate exit boundary condition, but only if you were already in the ballpark of the correct flow rate.

If your supersonic flow originated at the inlet, then you know for sure that your choice of inlet BC is to blame.

[mariconeagles96]

Originally Posted by the_phew

For most internal flows, you should use a total pressure inlet BC, and vary static pressure on the exit BC to achieve your desired flow rate (this is true in every CFD solver). Once you get through the startup transient, you can probably switch to a volumetric flow rate exit boundary condition, but only if you were already in the ballpark of the correct flow rate.

If your supersonic flow originated at the inlet, then you know for sure that your choice of inlet BC is to blame.

Thanks! Perhaps I'll try to use this method similar when doing windtunnel testing where you increase the pressure and jot down the corresponding flowrate.

Anyways. I tried the inlet flow rate setting with pressure static at exit without the rotation (just to check) and no problem at all with the mass balance. It seems when I turned this ON then solver have a difficult time to converge.

As for the supersonic flow, my internal analysis works just fine with those inlet vol fow rate. It's in the external analysis that this msg occurs. Lids are still there but just the domain (ext) was enlarge. I made this coz i was planning to do heat transfer with natural convection where my PCBA is attached to the water pump. If I do internal analysis I am forced to input heat transfer coefficient which I dont prefer.

Any thoughts? Appreciated it! Thanks! =)