Centrifugal Pump CFX convergence diffuculties
 

Hello,

I have convergence issues with the steady stade centrifugal Pump. The Momentum do not go under 10^-3. And the max. Residuals bouncy.

Measurement data of the pump at 1791 rev/min:

P_in: -19886Pa
P_out: 78775Pa

Model:
-Intake tube (length 150mm)
-Impeller (without gaps in front and behind the Impeller-->reduce Mesh elements)
-Volute

current Mesh:
-ca. 8 Mio Elements
-Assembly so I have a uniform Mesh
-10 Inflation Layer (total thickness 0,6mm, layer compression) (not automatic inflation, each Domain severel,also Interface e.g. from Impeller to volute inflated)
-curvature and wall distance
- elements in gap=8
-max element size=5mm
-min element size=0,1mm
max. skewness=0,91

Solver Settings:
operation Conditions 100344Pa
inlet: -19886Pa
outlet: mass Flow=3.86kg/s

Monitor Point:
Pressure Inlet: -19886Pa and Total Pressure= st. Pressure + Operating Pressure, so that is correct

no slip wall
SST-->with curvature correcction (recommanded for Centrifugal Pumps)
Time-Scale: I have try out: Auto-Time-Scale (0,0038s), pysical Time-Scale (1/omega) omega in rad/s or (1/(pi*rev/min)) or smaler (smalest Mesh Element/ (Tip speed r*omega) =0.000019s-->than it solves transient behavior, but small time-Scale give a more accurate Flow fild, this is required for turbulance equations....and so on.
Turbulance: 1. Order better for Tetraeder Mesh 2. Order

Solution:
-a higher Delta p -->Ansys calculatet an P_out: 1.2bar -->comparison Measurements 0.89bar.

but that is correct because I negligible friction losses for the rotating disc an gap losses too.

I have try out Velocity Inlet and Mass Flow outlet, that gives the same Delta p.

But the Residuals for the Momentum do not come down under 10^-4 after 300 til 600 iterations. And and the pressure distribution in the impeller is uneven for comparison to a Simulation only with the impeller.



I have tried so much, even with the model and smaller speed it will not get better. I need some help.

You have covered many of the issues discussed on the FAQ on this (But not all of them): http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Things you have not tried yet:
* Improve mesh quality (post an image of your mesh so we can see it)
* Try to assess whether the flow has transient flow structures
* Run it transient

how can I insert a picture?

the maximum residuals of conservation of momentum, which wobble, are in the Intake Domain by the Interface between Intake and Impeller/ hub. Which distance I take between the MRF (Impeller hub) and the intake

mesh intake and impeller
https://www.dropbox.com/s/v0j88og8b6...ntake.png?dl=0

mesh impeller and volute
https://www.dropbox.com/s/gxx4luvm88...olute.png?dl=0

mesh global
https://www.dropbox.com/s/s3mnq06afk...lobal.png?dl=0

residuals
https://www.dropbox.com/s/q81aiyzf9y...duals.png?dl=0

user point static pressure inlet and outlet
https://www.dropbox.com/s/3ju7kqgl2b...Point.png?dl=0http://www.cfd-online.com/Forums/G:\CFD online

Firstly: Your post has convinced me to updated the FAQ on posting images on the forum. The FAQ on this is now updated to show a far better way of uploading images to the forum: http://www.cfd-online.com/Wiki/Ansys...n_the_forum.3F

Secondly: Please do not PM me with CFD questions. If it is on the forum I will see it.

Finally: Your questions :)

Your mesh quality is not too good. That is likely to be the cause of convergence issues. The problem is the large change in size between adjacent elements, particularly where the inflation layers end to the first element in the bulk mesh. You need to make it so the volume of the last inflation layer is approximately equal to the volume of the element in the volume mesh it is next to.

ok, I will try,

an the boundary or inflation layer between the interfaces, is that a problem or equal for the solver?

I did it so because the automatic generation of inflation Layer do not work at the transition from impeller to volute. There he do not make a connection but stepstairs-->thats bad because of skeewnes

whats your meaning

I think I must try to generate the mesh with ICEM CFD and not with CFX ICEM

It is best not to put inflation layers on interfaces. Keep the mesh size similar along streamlines as far as you can.

sorry, I do not understand what "go advanced" what that is.

time scale
 

I have mange to mesh the hole model with the automatic inflation layer. And now I have a y plus of 1 til 10 on the impeller wall. Is it refine enough?

And whats better for steady state convergence in the pump. A bigger or smaler Time-Schale concrete bigger orsmaler than 1/omega ?

The problem I was talking about was not y+. It was the change in mesh size from the inflation layers to the volume mesh.

For the steady state time scale: Any of those numbers are a good starting point. From there you adjust it to suit. If it is converging consistently but slowly you increase the time scale; if it is converging poorly your decrease the time scale (but keep in mind the issues discussed in http://www.cfd-online.com/Wiki/Ansys...gence_criteria)

Mass Flow Inlet and Oulet
 

At boundary Condition:

is a Mass Flow Inlet and Mass Flow Outlet possible? When I only want to know the p2-p1

or better

Velocity Inlet and static Pressure Outlet?

You cannot have massflow inlet and outlet. Then:
a) the pressure is undefined, and
b) differences in massflow between the inlet and outlet (even tiny floating point rounding effects) cannot be accounted for and result in non-convergence.

Velocity inlet and static pressure outlet can work. But read the documentation on selecting boundary conditions in the CFX documentation for more advice on good selections.

How much iteration
 

And how much iteration are normal for my pump System ? About 200, 300, 400 or more?

That depends on the complexity of what you are simulating. For for a simple pump and single phase flow you should have convergence in under 100 iterations.

mass flow inlet and outlet
 

I have done a comparison with these conditions:

-Total Pressure Inlet and Mass Flow outlet
-Mass Flow Inlet and Mass Flow outlet

It gives the same delta P and the pressure and velocity contour look the same

new solutions
 

I have some pictures about my new solution with the new mesh.

what is your meaning about the convergence and the vector plot and the pressure contour plot, they look strange.

pressure contour plot
 

is that normal?

the pump
 

this pump is a little more complex than others

operating conditions
 

please a short explain.

I have relative measurements about the static pressure of the pump for i.g.:

-P_inlet: -19886 Pa
-P_outlet: 78775 Pa

In Ansys I set the Operation Pressure to 78775 Pa and the pump outlet a static Pressure to 0 Pa.

or

Ansys I set the Operation Pressure to 1 atm (or my measured ambient pressure 100344 Pa) and the pump outlet a static Pressure to 78775 Pa.

These are simple but important questions.

As your blades are simple and straight I would expect there to be large separations behind the blades. Also your outlet runner has a few wiggles which will also trigger separations. Both of these issues increase the complexity of the simulation and mean it will be harder to get convergence. So yes, your pump is a little more complex than normal. But not massively complex, it is quite manageable.

Your pressures mean a reference pressure of 100344Pa makes sense, then the inlet will be -19886 Pa and the outlet 78775 Pa.

no idea
 

- Is the mesh ok?

- whats your meaning about the velocity distribution?

- what I could check?