
[Sponsors] 
March 24, 2013, 09:39 
CFX fails to calculate a diffuser pipe flow

#1 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 7 
Sponsored Links
It seems so simple a problem, but CFX can't get convergency result! The attachment is the model picture and the CCL file. Could you give me some valuable advices on how to get a convergency result for this question? When the inlet velocity is less than 100m/s(approximately Mach Number 0.3), It easily gets convergency result, but when inlet velocity is more than 100m/s(approximately Mach Number 0.3), It can't get convergency result no matter how I adjust the calculation parameters. model.jpg mesh.jpg # State file created: 2013/03/24 21:10:03 # CFX14.0 build 2011.10.1023.01 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: Default Domain Coord Frame = Coord 0 Domain Type = Fluid Location = SOLID BOUNDARY: inlet Boundary Type = INLET Location = INLET BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Option = Static Temperature Static Temperature = 300 [K] END MASS AND MOMENTUM: Normal Speed = 200 [m s^1] Option = Normal Speed END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END END BOUNDARY: outlet Boundary Type = OUTLET Location = OUTLET BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Average Static Pressure Pressure Profile Blend = 0.05 Relative Pressure = 0 [atm] END PRESSURE AVERAGING: Option = Average Over Whole Outlet END END END BOUNDARY: wall Boundary Type = WALL Location = WALL BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END 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 = 1 [atm] END END FLUID DEFINITION: Fluid 1 Material = Air Ideal Gas Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Include Viscous Work Term = On Option = Total Energy END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = SST END TURBULENT WALL FUNCTIONS: High Speed Model = On Option = Automatic END END END OUTPUT CONTROL: BACKUP RESULTS: Backup Results 1 File Compression Level = Default Option = Standard OUTPUT FREQUENCY: Iteration Interval = 40 Option = Iteration Interval END END MONITOR OBJECTS: MONITOR BALANCES: Option = Full END MONITOR FORCES: Option = Full END MONITOR PARTICLES: Option = Full END MONITOR POINT: Monitor Point 1 Cartesian Coordinates = 0.2 [m], 0 [m], 0 [m] Option = Cartesian Coordinates Output Variables List = Velocity END MONITOR POINT: Monitor Point 2 Cartesian Coordinates = 0.3 [m], 0.01 [m], 0.02 [m] Option = Cartesian Coordinates Output Variables List = Temperature 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 COMPRESSIBILITY CONTROL: High Speed Numerics = On Total Pressure Option = Automatic END CONVERGENCE CONTROL: Length Scale Option = Conservative Maximum Number of Iterations = 500 Minimum Number of Iterations = 1 Timescale Control = Auto Timescale Timescale Factor = 1.0 END CONVERGENCE CRITERIA: Residual Target = 0.000001 Residual Type = RMS END DYNAMIC MODEL CONTROL: Global Dynamic Model Control = On END END END COMMAND FILE: Version = 14.0 END 

Sponsored Links 
March 24, 2013, 09:43 

#2 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 7 
================================================== ====================
OUTER LOOP ITERATION = 83 CPU SECONDS = 1.079E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  3.83  3.6E02  1.1E+00  2.0E02 OK  VMom  2.74  3.6E03  9.8E02  3.2E01 ok  WMom  2.80  3.6E03  8.0E02  3.2E01 ok  PMass  1.92  9.1E04  1.9E02  9.7 5.1E02 OK ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  1.05  6.2E03  1.8E01  6.3 4.2E03 OK ++++++  KTurbKE  0.93  1.9E02  3.3E01  6.3 1.0E03 OK  OTurbFreq  1.17  1.5E02  4.4E01  12.9 2.4E07 OK ++++++ ++  Notice: The maximum Mach number is 2.946E+00.  ++ ================================================== ==================== OUTER LOOP ITERATION = 84 CPU SECONDS = 1.092E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.57  2.0E02  2.3E01  3.8E02 OK  VMom  0.33  1.2E03  3.1E02  7.5E01 ok  WMom  0.32  1.2E03  2.8E02  8.3E01 ok  PMass  1.85  1.7E03  3.3E02  9.7 4.3E02 OK ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  0.79  4.9E03  2.1E01  6.2 1.6E02 OK ++++++  KTurbKE  0.75  1.4E02  2.4E01  6.2 1.1E02 OK  OTurbFreq  1.26  1.9E02  5.3E01  12.8 1.0E04 OK ++++++ ++  Notice: The maximum Mach number is 3.830E+00.  ++ ================================================== ==================== OUTER LOOP ITERATION = 85 CPU SECONDS = 1.105E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.85  1.7E02  2.3E01  4.8E01 ok  VMom  0.61  7.4E04  1.8E02  9.1E+00 F   WMom  0.59  6.9E04  1.8E02  1.0E+01 F   PMass  0.98  1.6E03  3.7E02  9.7 3.2E01 ok ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  0.93  4.5E03  1.3E01  6.2 1.0E02 OK ++++++  KTurbKE  1.42  2.0E02  2.7E01  6.2 2.0E03 OK  OTurbFreq  1.37  2.6E02  6.8E01  12.7 3.2E06 OK ++++++ ++  Notice: The maximum Mach number is 7.261E+00.  ++ ================================================== ====================  Timescale Information    Equation  Type  Timescale  ++++  UMom  Auto Timescale  2.50981E04   VMom  Auto Timescale  2.50981E04   WMom  Auto Timescale  2.50981E04   PMass  Auto Timescale  2.50981E04  ++++  HEnergy  Auto Timescale  2.50981E04  ++++  KTurbKE  Auto Timescale  2.50981E04   OTurbFreq  Auto Timescale  2.50981E04  ++++ ================================================== ==================== OUTER LOOP ITERATION = 86 CPU SECONDS = 1.117E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.18  3.1E03  4.6E02  1.1E+00 F   VMom  0.72  5.3E04  5.5E02  9.1E01 ok  WMom  0.78  5.4E04  4.8E02  1.0E+00 F   PMass  0.03  5.7E05  9.4E04  9.7 9.3E01 ok ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  0.81  3.7E03  1.0E01  6.2 3.0E04 OK ++++++  KTurbKE  1.17  2.3E02  3.1E01  6.2 1.5E04 OK  OTurbFreq  1.29  3.3E02  7.9E01  12.7 2.2E07 OK ++++++ ++  Notice: The maximum Mach number is 7.189E+01.  ++ ================================================== ==================== OUTER LOOP ITERATION = 87 CPU SECONDS = 1.130E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.03  9.7E05  5.7E03  2.8E01 ok  VMom  0.13  7.0E05  4.6E03  5.5E01 ok  WMom  0.13  7.0E05  4.7E03  6.0E01 ok  PMass  0.00  3.3E08  1.5E06  9.7 2.1E+01 F  ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  1.27  4.7E03  4.1E01  6.1 1.7E05 OK ++++++  KTurbKE  0.33  7.7E03  2.9E01  6.1 2.7E04 OK  OTurbFreq  1.40  4.7E02  1.0E+00  12.6 4.5E06 OK ++++++ ++  Notice: The maximum Mach number is 3.953E+03.  ++ ================================================== ==================== OUTER LOOP ITERATION = 88 CPU SECONDS = 1.142E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  3.04  2.9E04  1.6E02  9.5E03 OK  VMom  3.11  2.2E04  1.4E02  4.3E03 OK  WMom  2.91  2.0E04  1.4E02  5.3E03 OK  PMass  1.32  4.4E08  5.3E06  9.7 6.3E01 ok ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  0.62  2.9E03  4.9E01  6.0 5.0E05 OK ++++++  KTurbKE  0.91  7.0E03  2.1E01  6.0 3.0E03 OK  OTurbFreq  0.19  9.1E03  9.8E01  12.7 1.8E06 OK ++++++ Parallel run: Received message from slave  Slave partition : 3 Slave routine : get_TWFTFC Master location : End of Continuity Loop Message label : 009100015 Message follows below  : ++  ****** Notice ******   The nondimensional near wall temperature (T+) has been clipped   for calculation of Wall Heat Transfer Coefficient.     Boundary Condition : wall   T+ clip value = 1.0000E10     If this situation persists and you are using the High Speed Model,   consider enabling Mach number based blending between low speed and   high speed wall functions. You can do so by specifying a Mach   number threshold as follows:     EXPERT PARAMETERS:   highspeed wf mach threshold = 0.1 # default=0.0 (off)   END  ++ ++  Notice: The maximum Mach number is 1.254E+05.  ++ ================================================== ==================== OUTER LOOP ITERATION = 89 CPU SECONDS = 1.155E+03   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.00  6.4E08  7.8E06  1.8E02 OK  VMom  0.00  4.9E07  7.3E05  3.1E03 OK  WMom  0.00  4.0E07  7.3E05  4.4E03 OK  PMass  0.12  5.2E09  1.9E06  9.7 6.3E+00 F  ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 100.0% of the faces, 100.0% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Fluid 1.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++ ++  ****** Notice ******   The nondimensional near wall temperature (T+) has been clipped   for calculation of Wall Heat Transfer Coefficient.     Boundary Condition : wall   T+ clip value = 1.0000E10     If this situation persists and you are using the High Speed Model,   consider enabling Mach number based blending between low speed and   high speed wall functions. You can do so by specifying a Mach   number threshold as follows:     EXPERT PARAMETERS:   highspeed wf mach threshold = 0.1 # default=0.0 (off)   END  ++ Parallel run: Received message from slave  Slave partition : 2 Slave routine : get_TWFTFC Master location : RCVBUF,MSGTAG=1032 Message label : 009100015 Message follows below  : ++  ****** Notice ******   The nondimensional near wall temperature (T+) has been clipped   for calculation of Wall Heat Transfer Coefficient.     Boundary Condition : wall   T+ clip value = 1.0000E10     If this situation persists and you are using the High Speed Model,   consider enabling Mach number based blending between low speed and   high speed wall functions. You can do so by specifying a Mach   number threshold as follows:     EXPERT PARAMETERS:   highspeed wf mach threshold = 0.1 # default=0.0 (off)   END  ++ Parallel run: Received message from slave  Slave partition : 3 Slave routine : ErrAction Master location : RCVBUF,MSGTAG=1032 Message label : 001100279 Message follows below  : ++  ERROR #001100279 has occurred in subroutine ErrAction.   Message:   Floating point exception: Overflow            ++ 

March 24, 2013, 09:50 

#3 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 7 
But when I calculate this problem with FLUENT by import the CFX def file, FLUENT can give good convergency result when the inlet velocity is 200m/s, while still can't get convergency result when the inlet velocity is 300m/s.


March 24, 2013, 18:18 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,737
Rep Power: 106 
I see you have viscous heating on, I would turn that off unless you need it.
Other than that, the FAQ describes the steps to take: http://www.cfdonline.com/Wiki/Ansys...gence_criteria 

March 25, 2013, 06:43 

#5 
Member
Thiagu
Join Date: Oct 2012
Location: India
Posts: 59
Rep Power: 6 
Yes, flow is sub sonic and compressible.
At glance I don’t see any problem with BC. But not clear about initialization. Would recommend you initialize the domain only with Uvelocity of 200 m/s and fix the time step based on the residence time/10 (diffuser length , inlet velocity). 

March 25, 2013, 06:52 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,737
Rep Power: 106 
Viscous heating has nothing to do with subsonic or compressible flow. You only turn it on if the fricition/dissipation in the flow is generating heat and you care about it. This is not important in 99% of flows, so it should be turned off except if you are the 1% of flows where it is important.
Do not try to estimate residence time to get the time step. Maybe use it as a starting point, but adjust it from there based on how the simulation is going. If convergence is difficult then make it smaller, if converging easily then make it bigger. The time step you end up with is going to be quite different to anything you started with. Initialising with 200m/s is a starting point. If that works that is good. If that causes problems I would do a simulation at 100 m/s or 150 m/s and use that as an initial condition. Finally  this simulation looks axisymmetric. So why model it as 3D? Why not model it as a 2D axisymmetric wedge (http://www.cfdonline.com/Wiki/Ansys...tion_in_CFX.3F) 

March 25, 2013, 23:28 

#7 
New Member
Shen Ying
Join Date: Jan 2012
Posts: 22
Rep Power: 7 
Thanks, Glenn and Jthiakz.
I tried initialization, small time steps, and turning off Viscous heating, but none of them works. At last , I changed the inlet boundary condition to Total pressure inlet, just estimate a total pressure which can generate a inlet velociy near 200m/s， then it converges so quickly! Then I suddenly remember that in FLUENT velocityinlet is only suitable for incompressible flow. Maybe so is in CFX? just as I said before in this thread "When the inlet velocity is less than 100m/s(approximately Mach Number 0.3), It easily gets convergency result, but when inlet velocity is more than 100m/s(approximately Mach Number 0.3), It can't get convergency result no matter how I adjust the calculation parameters…" By the way, this simulation is indeed axisymmetric, so I will try a 2D axisymmetric wedge . Thank you for your good advice, Glenn. In fact, I often found that in those convergency result, there are asymmetry problems, for instance, the isoline of wall temperature are not axisymmetric. That's really confusing. 

March 26, 2013, 05:13 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,737
Rep Power: 106 
When you model it 2D axisymmetric you should be able to refine the mesh to a much higer degree, and achieve a much better mesh quality. This will assist convergence and accuracy.


Tags 
diffuser pipe flow 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Compressible Flow in Ansys CFX  bcheruk  CFX  15  July 6, 2017 06:30 
integral length scale and crosscorrelation (with openfoam data, LES pipe flow)  jet  Main CFD Forum  1  November 7, 2016 05:23 
[ASK] Flow in Corrugated Pipe with FLUENT  Primadhani  FLUENT  1  May 11, 2011 20:41 
fluid flow fundas  ram  Main CFD Forum  5  June 17, 2000 21:31 
Hydrostatic pressure in 2phase flow modeling (long)  DS & HB  Main CFD Forum  0  January 8, 2000 16:00 
Sponsored Links 