[ngoc_tran_bao]

Dear all,
I'm carrying out a pump simulation and try to plot velocity vector at mid plane of impeller passage in order to visualize jet-wake structure. This is the phenomenon which occurs near suction side of impeller blade due to low velocity flow. However, the result observed from simulation is different from theoretic researches. The low velocity region should be appeared in suction side of blade, but in my case it is on pressure side (as in enclosed picture). I do not understand why my simulation is reverse. Do my set up in CFX-pre have somethings wrong? Can anyone give me some points?
Thank you for reading my thread.
Here is my CELownload URL:http://www.gigasize.com/get/6zxwp7fz0pc

[alirezame]

Hello,

Please mention your boundary condition and all settings you did in CFX-pre.

[Opaque]

Have you looked into the plots for Velocity in Stn Frame ?

[ngoc_tran_bao]

Hi Lirezame,
As for BC, I set total Pressure at Inlet = 0.14 Mpa;
Mass Flow rate at Outlet = 80 m3/h;
Rotation = -1750 RPM (Z axis)
Smooth wall for all suction, discharge walls;
Reference Pressure =0 atm;
Physical time step =1/W.
You can look for detail in my CEL in the thread.

[alirezame]

can you put a figure of your CEL? the link does not work properly.

[ngoc_tran_bao]

Hi Opaque, thank for your suggest.
I get the same result with velocity in stationary frame. Like this picture:

[ngoc_tran_bao]

This is CEL of my simulation, can you help me to take a look. I hope it's not too long, thank you.
ANALYSIS TYPE:
Option = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Discharge
Coord Frame = Coord 0
Domain Type = Fluid
Location = DISCHARGE_FLUID_1_1_SOLID
BOUNDARY: Discharge_wall
Boundary Type = WALL
Location = DISCHARGE_WALL
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Impeller_discharge Side 2
Boundary Type = INTERFACE
Location = DISCHARGE_IN
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Outlet
Boundary Type = OUTLET
Location = OUTLET
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 17.0666667 [kg s^-1]
Option = Mass Flow Rate
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 25 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
Option = Scalable
END
END
END
DOMAIN: Impeller
Coord Frame = Coord 0
Domain Type = Fluid
Location = ROTATING_FLUID_CHUAN_1_1_SOLID
BOUNDARY: Blade
Boundary Type = WALL
Frame Type = Rotating
Location = BLADES,HUB,SHROUND
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Impeller_discharge Side 1
Boundary Type = INTERFACE
Location = IMPELLER_OUT
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Impeller_wall
Boundary Type = WALL
Frame Type = Rotating
Location = IMPELLER_WALL
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
WALL VELOCITY:
Option = Counter Rotating Wall
END
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Intake_Impeller Side 2
Boundary Type = INTERFACE
Location = IMPELLER_IN
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Alternate Rotation Model = On
Angular Velocity = -1750 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 25 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
Option = Scalable
END
END
END
DOMAIN: suction
Coord Frame = Coord 0
Domain Type = Fluid
Location = INTAKE_BULKHEAD_EXTEND_1_1_SOL
BOUNDARY: Inlet
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = 0.14 [MPa]
END
TURBULENCE:
Option = Low Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: Intake_Impeller Side 1 1
Boundary Type = INTERFACE
Location = INTAKE_OUT
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Intake_wall
Boundary Type = WALL
Location = INTAKE_WALL
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Water
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 25 [C]
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
Option = Scalable
END
END
END
DOMAIN INTERFACE: Impeller_discharge
Boundary List1 = Impeller_discharge Side 1
Boundary List2 = Impeller_discharge Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Frozen Rotor
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = Specified Pitch Angles
Pitch Angle Side1 = 360 [degree]
Pitch Angle Side2 = 360 [degree]
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Suction_Impeller
Boundary List1 = Intake_Impeller Side 1 1
Boundary List2 = Intake_Impeller Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Frozen Rotor
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = Specified Pitch Angles
Pitch Angle Side1 = 360 [degree]
Pitch Angle Side2 = 360 [degree]
END
END
MESH CONNECTION:
Option = GGI
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: P outlet
Coord Frame = Coord 0
Expression Value = areaAve(Pressure)@Outlet
Option = Expression
END
MONITOR POINT: Torque
Coord Frame = Coord 0
Expression Value = torque_z@Blade
Option = Expression
END
MONITOR POINT: Vel outlet
Coord Frame = Coord 0
Expression Value = areaAve(Velocity in Stn Frame)@Outlet
Option = Expression
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Iterations = 2000
Minimum Number of Iterations = 1
Physical Timescale = 0.01 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Residual Target = 1e-04
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END

[alirezame]

did you get fully converged calculation? according to the residual target which is a bit large and your time step, maybe your result has not converged yet.
what were your convergence criteria?

[ngoc_tran_bao]

Dear Alirezame,
For this simulation, I got the convergence. You mean the convergence criteria of 10^-4 is large, so I need to reduce it to somewhere around 10^-5 in order to get higher accuracy? May be, you're right, but in most of the paper I have read, researchers often used a convergence criteria of 10^-4 and I think it is enough.

[alirezame]

''Residual Target = 1e-04'' it means that once one of the residuals reaches this amount, solver stops and gives to the convergence notification even before the maximum number of iteration. In most of cases, RMS P-Mass comes lower than other RMS residuals and this affects the accuracy by selecting 10^-4 as the residual target. in my opinion, decrease the residual target to 10^-8 o even lower and check the imbalance of all zones (as you know it should be too close to zero and stable) and also stability of the efficiency instead of residual checks.
other settings seem correct in my opinion.

[ngoc_tran_bao]

Thanks, I have never used such a low convergence target of 10^-8. I will try to reduce it as you suggest, and will post result if it work. Thank you, again.

[-Maxim-]

Originally Posted by alirezame

''Residual Target = 1e-04'' it means that once one of the residuals reaches this amount, solver stops

As far as I understood, ALL residuals have to be lower than that number.
I always use MAX residuals, but I don't think RMS is different.
I also don't think 10^-4 is the culprit here...

15.10.1.1.1. RMS Residual Level




Although the required convergence level depends on the model and on your requirements, the following guidelines regarding RMS residual levels may be helpful.

• Values larger than 1e-4 may be sufficient to obtain a qualitative understanding of the flow field.
• 1e-4 is relatively loose convergence, but may be sufficient for many engineering applications. The default target RMS residual value is 1e-4.
• 1e-5 is good convergence, and usually sufficient for most engineering applications.
• 1e-6 or lower is very tight convergence, and occasionally required for geometrically sensitive problems. It is often not possible to achieve this level of convergence, particularly when using a single precision solver.

15.10.1.1.2. MAX Residual Level




MAX residuals are typically 10 times larger than the RMS residual; The above guidelines for RMS residuals can also be applied to MAX residuals, with the targets increased by a factor of 10.
Sometimes, however, the MAX residuals are much larger (for example, a factor of 100) than the RMS residuals. In this situation, it is very likely that the region of high MAX residuals is isolated to a very small area of the flow, typically where some unstable flow situation exists (for example, a separation or re-attachment point, and so on). It may be the case that this small area of unstable flow / lack of tight convergence of the MAX residuals do not affect the overall prediction. To verify that the solution is acceptable, you should verify that the variation of relevant quantities (for example, lift, drag forces, efficiency of the device, and so on) is small.

Release 17.0 - © SAS IP, Inc. All rights reserved.

Are your imbalances under 1%?
I would not use a specific mass flow rate at the outlet. The impeller is supposed to create the mass flow and not the boundary conditions.

[ngoc_tran_bao]

Maxim: I do not really understand the terminology "imbalance" you referred to. As for Outlet BC, many tutorials guide learners to set Flow rate at Outlet. It is more seasonable than Pressure. So I dont think it make me get trouble. In your opinion, what should we set for outlet BC?

[ghorrocks]

MAX vs RMS: The equation residuals are calculated at each integration point. Over the entire domain you can take either the RMS or MAX value as your convergence criteria. Obviously RMS is looser, and will allow a small number of points to have large residuals but still achieve convergence. MAX means that no integration point exceeds the criteria so is much stricter. MAX can be hard to use in poor quality meshes as the residuals in the poor mesh regions will be much higher than everywhere else.

1e-4: Yes, this is guide to convergence but only a guide. You should do a sensitivity check to establish what criteria you need for adequate convergence.

Imbalances: This looks at the global conservation of things like mass, momentum and heat. For instance the total mass flowing into the domain must equal the mass flowing out in steady state; or the momentum across a domain must sum to zero and so on. For simulation where these global balances are important including imbalances in your convergence criteria is a good idea (eg CHT simulations). But flow over an airfoil is an example of a flow where it probably is not required as the residuals are a good guide to convergence.

Which Boundary Condition: You should use boundary conditions which match what you know about the flow. If you know the flow rate then use a velocity, If you know the pressure then use a pressure boundary. If you don't know anything then you can't put a boundary there and must move the boundary to somewhere where you do know the flow conditions.

[ngoc_tran_bao]

Ghorrocks, thank you Sir, I learn a lot from your reply.
As for BC: I have already known the total pressure at Inlet, Head and Q design of the pump, now I try to investigate vector velocity of flow field in different flow rates (both design and off-design condition). That's the reason why I set Flow rate for Outlet BC and vary it for each circumstance.
As for imbalance: as I understand, in my case if I put an flow rate at outlet, after getting the solution I need to check flow rate at Inlet to compare it. Is this right? I have done this, the discrepancy is quite small, about 0.0245%.
What I wonder in my result is that, the low velocity region should be appeared in suction side of blade, but in my case it is on pressure side. Can you give me some ideas about this abnormal phenomenon?

[-Maxim-]

Originally Posted by ngoc_tran_bao

As for imbalance: as I understand, in my case if I put an flow rate at outlet, after getting the solution I need to check flow rate at Inlet to compare it. Is this right? I have done this, the discrepancy is quite small, about 0.0245%.

In Solver Manager, you add a new monitor and add as Plot Line Variable all of the Imbalances (P-Mass, U-Mom, V-Mom, W-Mom). As a general rule: They should be less than 1%.

[ngoc_tran_bao]

Originally Posted by -Maxim-

In Solver Manager, you add a new monitor and add as Plot Line Variable all of the Imbalances (P-Mass, U-Mom, V-Mom, W-Mom). As a general rule: They should be less than 1%.

Oh, I get it. Unfortunately, the imbalance in Impeller and discharge domain are upto 10%. That's so bad.

[turbo]

The tolerance of 1e-4 would be OK if not so accurate solution is wanted for check. From what view do you say "Low velocity happens on the pressure side" ??? I do not get it.

[ngoc_tran_bao]

Originally Posted by turbo

From what view do you say "Low velocity happens on the pressure side" ??? I do not get it.

Hi, Turbo. You can see on the 1st picture, there are short vectors in dark blue which indicate low velocity flow at pressure side of blade. Meanwhile, at suction side the appearance of long,light blue vectors which indicate high velocity is observed.

[ngoc_tran_bao]

Maxim, I think I get high imbalance in this circumstance because I carry out the simulation at off-design condition ( Q=0.6 Qdesign). Another simulation at design condition gives me quite low imbalance, all imbalances are under 1%. However, the abnormal phenomenon of low velocity flow field still exists. I think there is something wrong in setup parameters but I can not find it.