
[Sponsors] 
Convergence problem of CFX when comparing with FLUENT with same mesh 

LinkBack  Thread Tools  Display Modes 
May 22, 2014, 11:40 
Convergence problem of CFX when comparing with FLUENT with same mesh

#1 
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
Hi, all,
Thank you for reading my post. I am carrying comparison of 2D simulation between CFX and FLUENT. Results from FLUENT agrees well with experiments (residuals reduce to 3E7). But CFX results only have residuals of 5E5, with same mesh and setting. The lift and drag coefficients in CFX are near to FLUENT results and experimental data. But the turbulence intensity decay too fast in CFX. The intermittency have a total different distribution compared with FLUENT, with intermittency=1 in free space. How can I reduce the residual of CFX? Why I have a different turbulence intensity and intermittency distribution in CFX? Here is the detailed question: Validation of lift and drag for airfoil AerospatileA, chord=1m, attack angle=13, exterior flow, Inlet velocity=51, Re=1E7. Mesh: size=194720, O Grid, Y+<1 Model: SST transition FLEUNT CASE: boundary condition INLET: Ux=51 m/s (Uy=Uz=0), intermittency=0, turbulent intensity=0.3%, turbulent viscosity ratio=35. The left line, the top line and down line are both considered inlet. SOLUTION METHODS SIMPLE, Green Gauss Node Based, Secondorder upwind for other discretization The residuals and turbulence intermittency and intensity are shown in attached files. The maximum intermittency is 1, with free space intermittency=0. The intensity decay from inlet to leading edge, from 0.298% to 0.278%. 

May 22, 2014, 11:48 

#2 
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
CFX CASE
In order to carry out the 2d simulation, we extruded the same 2d mesh for one element thickness, only one layer in Z direction. Boundary condition INLET: turbulence intermittency in GUI cannot be set. We edit in Command Editor, with specified inlet intermittency, velocity, intensity and viscosity ratio. ================================================== ======== MASS AND MOMENTUM: Option = Cartesian Velocity Components U = 51.46714 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END TRANSITIONAL INTERMITTENCY: Intermittency = 0 Option = Value END TURBULENCE: Eddy Viscosity Ratio = 35 Fractional Intensity = 0.003 Option = Intensity and Eddy Viscosity Ratio END ============================================== Boundary Condition for Top and Bottom surfaces in extruded mesh: Symmetric Fluid Model SST gammatheta (shown in pics) CFX RESULTS: only have a residual of 6e5. Turbulence intermittency The Maximum is 2. For the free space, it is filled by intermittency=1. However, in Fluent results, the maximum is 1. The free space is filled by intermittency=0. It is very strange. (shown in attached files) Turbulent intensity from inlet to the leading edge Decay too fast. Only 0.13% for leading edge. While in Fluent, it is 0.278% for leading edge. (shown in attached files) 

May 22, 2014, 11:58 

#3 
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
I would appreciate if anyone can help me.
Thank you! 

May 22, 2014, 12:45 

#4 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11 
Not sure what your problem is. You are getting matching answers to experiment from both CFX and Fluent. Well Done!
1) You shouldnt be trying to compare residual magnitudes between codes. That is meaningless. 2) Apparently the parameter you are worried about, turbulence and intermittancy, is not a big player in on the items (Cl and Cd) you are comparing to experiment. At least not at the level of the codes predicting different values and their impact on Cl and Cd. 3) You are failing in pressure in the linear solver in CFX. Be careful. 

May 22, 2014, 12:54 

#5  
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
Thank you for your reply. My question is that how can I reduce the residuals, then I can trust the results. At least 1E6.
Yes, pressure in the linear solver sometimes failed, and Umom, Vmom also failed. How can I solve this problem？ Thank you very much! Quote:


May 22, 2014, 13:02 

#6 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11 
Do not look to residuals to "trust" your results. Are you matching experimental data or aren't you? If you are, then you're golden.
In industry, you often will not make models that drive the residuals way down. But you can make models with compromise, monitor the values you are really interested in, run the analysis to drive them to a suitable convergence, and call it good. Comparison to experimental data then tests your level of trust, not residuals. If you insist on driving the residuals down, check your inputs and improve your mesh. One or the other is not suitable to what you are modeling to drive the residuals down to the level you want. 

May 22, 2014, 14:29 

#7 
Senior Member
Join Date: Jun 2009
Posts: 311
Rep Power: 10 
From the FLUENT setup it is not clear if you are using second order discretization for all the equations (including turbulence), or only mass/momentum and energy. In your CFX setup, it is explicit you are using High Resolution for all of them (including turbulence).
Are you running single or double precision ? There are differences in how FLUENT and CFX normalize their residuals; therefore, do not focus on the exact values between the two codes, but the meaningful quantities for the problem at hand. How much relative extrusion did you apply on the CFX setup ? That is, how thick is your 2D model respect to the characteristic length of the problem. 

May 22, 2014, 14:37 

#8  
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
Quote:
For FLUENT, it is double precision. But for CFX, it is single precision. I can try double precision later to check the difference. Does it matter so much? For the 2D mesh, the whole domain is 100mX 120m, the airfoil in the middle is 1m chord. The thickness is 0.01m for extruded mesh. I also try 0.005m, but it doesnot change much for results. 

May 22, 2014, 15:13 

#9  
New Member
xin
Join Date: Dec 2013
Posts: 18
Rep Power: 3 
Quote:
Actually when I reduce the timescale in CFX, 0.01s, the linear solver works fine. Maybe this is one way to avoid the failure in linear solver. 

Tags 
cfx, fluent, turbulence intensity, turbulence intermittency 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
CFX convergence problem simulating ogivecylinders at varied angle of attack  jdacosta  CFX  6  February 25, 2015 22:42 
Comparison of fluent and CFX for turbomachinery  Far  CFX  52  December 26, 2014 19:11 
Mesh and Solve Times for CFX, Fluent, CDadapco  Jade M  Main CFD Forum  4  August 28, 2012 02:54 
[ICEM] Problem making structured mesh on a surface  froztbear  ANSYS Meshing & Geometry  4  November 10, 2011 09:52 
[ICEM] Problem making structural mesh on a surface  froztbear  ANSYS Meshing & Geometry  1  November 10, 2011 09:52 