[j0hnny]

Hi my frineds,

I am starting to simulate a CENTRIFUGAL FAN in ANSYS CFX 15

I want to calculate the efficiecy depending on the number of blades.

I have made the rotor with SW14 and and saved in IGES format to import into ansys.



I have many questions, first I simulate in ansys with the rotor (left image) or the inside with the flow (right image)?



Second, When import(in step, iges, etc. format) the rotor is broken in half. Why? Its normal?



3. Do I need to create a volute If yes, Why? in SW? Ansys?

I have made some experiencies, this is right?






please nyone can help me answering the doubts? I'm completely lost.

Regards

j0hnny

[ghorrocks]

Sounds like you should:

* Do the CFX tutorials which are provided with the software. Several of these are for rotating machinery. See the documentation under the help options.
* Read the best practices guides in the CFX documentation. There is one for rotating machinery.

[tomson199]

Hi
In the past I made some simulation of this type of rotating machines. First of all, if you try do do a comparison between experimental data and numerical simulations, you should build a CAD model similar to the test stand. This fan mostly work in the volute, because the efficiency of this machine is the highest then. The leakage offten occured in this situation, because generally we suck the air by the pipeline. Then you should take into account this phenomena. In the rotating machines, there is always efficiency peak. In this point the influence of blades number is less importance on efficiency. But when you lead fan to the stall, then this is significant, because the secondary loss and profile loss will be arise.

Take into account inlet and outlet angles of the blade. The ralative velocity should be always tangential, when you look for improve efficiency.

[j0hnny]

Hi, Thanks for the answers
I have read tutorials about turbomachinery and I have learned a lot

I defined boundary conditions for the rotor, volute and pipe
Interfaces between Pipe and rotor and between rotor and volute





But this error appears when trying to run my simulation:

Update failed for the Solution component in Fluid Flow (CFX). The solver failed with a non-zero exit code of : 2

+--------------------------------------------------------------------+
| Job Information at Start of Run |
+--------------------------------------------------------------------+

Run mode: partitioning run

+------------------------------+------+--------+----------+----------+
| Host | Mesh | PID | Job Started |
| | Part | | DD/MM/YY | hh:mm:ss |
+------------------------------+------+--------+----------+----------+
| JOAO | 1 | 9972 | 24/11/15 | 20:24:55 |
+------------------------------+------+--------+----------+----------+


+--------------------------------------------------------------------+
| Memory Allocated for Run (Actual usage may be less) |
+--------------------------------------------------------------------+

| Real | Integer | Character | Logical | Double
----------+------------+------------+-----------+----------+----------
Mwords | 2.55 | 7.35 | 3.38 | 0.12 | 0.00
Mbytes | 19.42 | 28.04 | 3.22 | 0.46 | 0.00
----------+------------+------------+-----------+----------+----------


+--------------------------------------------------------------------+
| Host Memory Information (Mbytes) |
+--------------------------------------------------------------------+
| Host | System | Allocated | % |
+-------------------------+----------------+----------------+--------+
| JOAO | 4077.86 | 51.14 | 1.25 |
+-------------------------+----------------+----------------+--------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Zero divide |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine FPX: C_FPX_HANDLER |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX partitioner exited with return code 1. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

Can someone explain me what should I do to make it work.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[tomson199]

Your model in preprocessor looks good. I think, that you did some small mistakes somewhere. Could you paste a CFX Command Language for Run from CFX Solver? There are described in details your boundary conditions. I will look them closer and try to help you

[j0hnny]

I have checked the proprieties of material, mesh, etc and i didnt found the possivel mistakes

Tomson199, if you dont mind checking CFX Command Language, I will be very grateful

+--------------------------------------------------------------------+
| |
| CFX Command Language for Run |
| |
+--------------------------------------------------------------------+
LIBRARY:
COORDINATE FRAME DEFINITIONS:
COORDINATE FRAME: Coord 1
Centroid Type = Absolute
Invert Normal Axis Direction = Off
Location = F20.18
Option = Point and Normal
Origin = -0.677829 [m], 0.215714 [m], -0.184879 [m]
Point on Axis 3 = -1.67783 [m], 0.215714 [m], -0.184879 [m]
Point on Plane 13 = 1 [m], 0 [m], 0 [m]
Reference Coord Frame = Coord 0
END
END
MATERIAL: Air at 25 C
Material Description = Air at 25 C and 1 atm (dry)
Material Group = Air Data,Constant Property Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1.185 [kg m^-3]
Molar Mass = 28.96 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-02 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 0.003356 [K^-1]
END
END
END
END
FLOW: Flow Analysis 1
SOLUTION UNITS:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
Option = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: Intake
Coord Frame = Coord 0
Domain Type = Fluid
Location = B18
BOUNDARY: Intlet
Boundary Type = INLET
Location = F20.18
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = 183 [Pa]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: intake to rotor Side 1
Boundary Type = INTERFACE
Location = F24.18
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: parede_intake
Boundary Type = WALL
Location = F21.18,F22.18
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: parede_interna
Boundary Type = WALL
Location = F562.18
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: Air at 25 C
Material = Air at 25 C
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: Volute
Coord Frame = Coord 0
Domain Type = Fluid
Location = B70
BOUNDARY: Rotor_volute Side 2
Boundary Type = INTERFACE
Location = F77.70,F78.70
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Volute Default
Boundary Type = WALL
Location = F565.70,F566.70,F567.70
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: parede_volute
Boundary Type = WALL
Location = F86.70,F84.70,F79.70,F564.70
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: saida_volute
Boundary Type = OUTLET
Location = F73.70
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 0.5101 [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: Air at 25 C
Material = Air at 25 C
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: rotor
Coord Frame = Coord 0
Domain Type = Fluid
Location = B332
BOUNDARY: Disco frontal_Shroud
Boundary Type = WALL
Frame Type = Rotating
Location = \
F352.332,F349.332,F345.332,F344.332,F343.332,F293. 332,F304.332,F299.3\
32,F297.332,F294.332,F329.332,F330.332,F331.332,F3 33.332,F338.332,F33\
5.332
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Disco traseiro_hub
Boundary Type = WALL
Frame Type = Rotating
Location = F334.332
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Rotor_volute Side 1
Boundary Type = INTERFACE
Location = F295.332,F346.332
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: intake to rotor Side 2
Boundary Type = INTERFACE
Location = F328.332
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: pas_blades
Boundary Type = WALL
Frame Type = Rotating
Location = \
F296.332,F298.332,F300.332,F301.332,F302.332,F303. 332,F305.332,F306.3\
32,F307.332,F308.332,F309.332,F310.332,F311.332,F3 12.332,F313.332,F31\
4.332,F315.332,F322.332,F321.332,F316.332,F317.332 ,F318.332,F319.332,\
F320.332,F323.332,F324.332,F325.332,F326.332,F327. 332,F336.332,F337.3\
32,F339.332,F340.332,F341.332,F342.332,F347.332,F3 48.332,F350.332,F35\
1.332,F353.332
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:
Alternate Rotation Model = true
Angular Velocity = 1369 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.1
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [atm]
END
END
FLUID DEFINITION: Air at 25 C
Material = Air at 25 C
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: Rotor_volute
Boundary List1 = Rotor_volute Side 1
Boundary List2 = Rotor_volute 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: intake to rotor
Boundary List1 = intake to rotor Side 1
Boundary List2 = intake to rotor 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:
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 1000
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Conservation Target = 0.01
Residual Target = 0.00001
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END
COMMAND FILE:
Version = 15.0
Results Version = 15.0.7
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = On
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: joao
Host Architecture String = winnt-amd64
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Independent Partitioning
Runtime Priority = High
EXECUTABLE SELECTION:
Use Large Problem Partitioner = Off
END
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
Partition Weight Factors = 0.25000, 0.25000, 0.25000, 0.25000
END
END
RUN DEFINITION:
Run Mode = Full
Solver Input File = Fluid Flow CFX.def
END
SOLVER STEP CONTROL:
Runtime Priority = Idle
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARALLEL ENVIRONMENT:
Number of Processes = 4
Start Method = Platform MPI Local Parallel
Parallel Host List = joao*4
END
END
END
END

I dont know if it's important to put the static pressure = 170 pa
I just put the total pressure = 183pa

[ghorrocks]

In the rotating domain you have "Alternate Rotation Model = true". You probably don't want that, turn it off. Also if you are having problems with convergence you don't want to use the auto time scale. You will need to use smaller time steps (as the FAQ says).

The problem is most likely to be your mesh quality (As the FAQ said - did you read it? Your question really has been asked a thousand times before). Please post an image showing a cross section through your mesh.

[tomson199]

I see that you use reference pressure 0 atm. On the first attempt, switch your energy model to none, because compressibility effects is negligible and pressure increase is relatively small. It might be wrong with Isothermal model and it produce values close to zero. Put the reference pressure equal 1 atm. In the test stand I am in 99% sure, that you analyze this machine in ambient condition. I think that it is the most possible cause of your problem. Next things is your boundary condition. In the real test stand you have after outlet any pipe or air from this place run out to the atmosphere? If yes, try to use massflow on the inlet and static pressure on the outlet. Last thing is pitch on the interfaces. On the both sides of them, you have a full 360 deg revolution of area, so change this option to NONE. When I starded my adventure in CFD, in the first attempts I used very badly mesh and despite this my calculations were made.

Sorry for my english, I practise my language every day to improve my communication

[ghorrocks]

Hi Thomas:

The model is isothermal. It is not modelling compressible flow, it is an incompressible flow model.

Your other points are correct, well spotted.

[tomson199]

I admit, I tell wrong with this Isothermal model.

Thanks Glenn

[j0hnny]

Thanks you a lot and i'm sorry not to have answered earlier.
I've been writing the thesis, and only now i returned to the part of the simulation.
Now works so well with your help

But I have some doubts. Is it normal those streamlines recede backwards? As illustrated in the next image.









I dont know why, but it seems the simulation is wrong. I have tried other ways, for example only the rotor, and already seem right.

[tomson199]

I'm happy, that you did it It is normal, that some streamlines go back through leakage, because there is a difference of pressures. You can minimilize thaht by minimize the gap in the leakage seal.

[ghoshi1983]

In case anybody interested in centrifugal/radial fan simulation here you can download (.res file) and have a look at it:
https://fetchcfd.com/view-project/39-Radial-Fan