
[Sponsors] 
April 21, 2005, 07:32 
>What OpenFOAM version are you

#21 
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8 
>What OpenFOAM version are you running?
1.1 >What solver? rhoTurbFoam >What thermodynamics package? // Thermophysical model thermoType hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>; mixture air 1 28.9 1300 2.544e+06 1.84e05 0.7; >Have you tried changing the gradient? >Does it run if the gradient is small enough? >Have you tried changing the sign of the >gradient? No I didn't try. I will, and I'll let you know, Thanks, Daniele 

April 21, 2005, 07:35 
I have checked the thermo libr

#22 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
I have checked the thermo library and the error in the thermodynamics only related to certain combustion thermo packages not the basic ones used by rhoTurbFoam.
Another useful check would be if you were to run with an isothermal wall and increase it's temperature and see what happens. 

May 19, 2005, 05:40 
Dear all,
I am using rhoTur

#23 
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8 
Dear all,
I am using rhoTurbFoam (URANS) for simulating a heated air pipe flow with high amplitude pulsation of the flowrate. Im using the following BC Inlet: prescribed pulsating velocity, gradient of p = 0, temperature inlet constant. Outlet: gradient of velocity = 0, gradiet p = 0, gradient T = 0 Wall: Twall = constant I am comparing Low Reynolds and High Reynolds Turbulence models. I would like also to change the wall functions. I have some questions: 1) rhoTurbFoam uses the turbulence models in src/turbulencemodels/compressible or incompressible ? 2) what is G in (compressible) wallDissipationI.H? is it the integrated contribution of epsilon in the near wall cell in the UMIST approach? 3) why the boundarySource of epsilon is multiplied by 1.0e+10? Daniele 

May 19, 2005, 05:46 
1) src/turbulencemodels/compre

#24 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
1) src/turbulencemodels/compressible
2) G is the turbulent kinetic energy generation rate (take a look at the sources in the kequation) 3) In wall function approaches epsilon is usually fixed in the nearwall cell and multiplying the source by a large number and setting the centralcoefficient to that number is a clunky but effective way of doing this. 

May 20, 2005, 03:32 
Thanks for the usefull explana

#25 
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8 
Thanks for the usefull explanation,
I have another question, I am experiencing problem in convergence when the amplitude of the pulsating flow in the channel is high, and I have reverse flow... the Co goes up and then I get the error message as Jarrod. Can be due to the BCs I am using? Schall I use inletOutlet and OutletInlet BC? If yes can somebody explain me how this BC works? In the manual it is written that using those BCs two value should be given, inletValue and value, what are they? Daniele 

May 20, 2005, 04:01 
Do you have outflow at the inl

#26 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Do you have outflow at the inlet or inflow at the outlet or both?
The inletOutlet BC simply changes the boundary condition for stability based on the direction of the flux, i.e. uses zerogradient for outflow and the value specified to inflow. outletInlet is the opposite which I created for pressure but it is unlikely to be appropriate in your case. I do not know what inflow value you should specify, do you know what the inflow should be? If you want to limit the reverse flow try specifying a zero inlet value. 

May 20, 2005, 05:18 
It is a pulsating channel, it

#27 
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8 
It is a pulsating channel, it means that I have both conditions, the inlet at some point becomes an outlet and the outlet an inlet.
I prescribe an oscillating value of velocity at the inlet and a fix value of pressure at the outlet.. I am not sure that this BCs are consistent.. Do you have any suggestions? Daniele 

May 20, 2005, 05:32 
You can use inletOutlet for th

#28 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
You can use inletOutlet for the velocity and outletInlet for the pressure but you will have to adjust the inlet value of velocity according to the way in which you are driving the pulsations.


May 20, 2005, 05:58 
Do you think that the BCs I wa

#29 
Senior Member
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8 
Do you think that the BCs I was giving are badposed or refining the grid and using a smaller time step can help?
Since I have already an oscillatingFixedValue BC, can I derive an inletOutletOscillatingFixedValue BC? Can you give me some hint on how to do that? where is the src of the inletOutlet BC ? Thanks for your time, Daniele 

May 20, 2005, 06:07 
Having boundary conditions tha

#30 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Having boundary conditions that change the bulk direction of the flow is likely to give problems and if you can think of ways to setup the case to avoid such complex and critical BCs it would be good idea.
You will find the implementation of the complex physical BCs in OpenFOAM1.1/src/OpenFOAM/fields/fvPatchFields/derivedFvPatchFields 

May 22, 2005, 23:37 
Hi Guys
I'm looking for the

#31 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hi Guys
I'm looking for the case root directory entry of rhoTurbFoam tutorials into foamX without success? Should I do something more to see the case root directory rhoTurbFoam tutorial dirs into the foamX trees? I guest that only if I can see this directory I should to edit and clone the case of rhoturbfoam class using foamX, is it? Many tanks in advance Wladimyr 

May 23, 2005, 16:09 
Hello Guys
I have got the s

#32 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hello Guys
I have got the same problem reported by Jarrod at MArch/17  item 1. It means, the solver crashes with the following message:> FOAM FATAL ERROR : Maximum number of iterations exceeded Function: specieThermo<thermo>:... How can I solve this problem? The test case is a NACA profile discretized in 3D. The spanwise is 3 mts and the cord is 1 m. The BC in the root and tips plane is simmetry (empty). The Mach is 0.7 and the farfield is divide in two parts: I defined the front farfield faces as inlet and the back farfield faces as outlet. Which are the best BC for farfield boundaries in such type of test case? And what means R in the fields? Is the Reynolds Stresses? Using the Kepsilon model, have I impose some value or it is calculated from the flowfield? Could someone help me? Many tanks in advance! Wladimyr Mattos Dourado 

May 23, 2005, 16:12 
Have you tried running incompr

#33 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Have you tried running incompressible?
Yes R is the Reynolds stress and is not used unless you choose a Reynolds stress model. 

May 24, 2005, 12:26 
Hi Weller
I initialy tried

#34 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hi Weller
I initialy tried to run the compressible solver rhoturbfoam. The last message is results of this temptative. Just now I run the incompressible solver (turbfoam) and its work. Why your question about to try the incompressible? How solve that problem (crashing due thermophysical function)? Second, I have the results of the incompresible solve. How can I transfer this field for the compressible case to use as initial conditions? The only way that I see now is copying the field files to the new comrpessible case first time directory. Have it another way to make this transfer using some foam tool ? Really opem Foam is a nice CFD code. COngrutulations for you initiative and soo I hope to colaborate more actively to develop new features for foam. Tank in advance for your help Wladimyr 

May 26, 2005, 13:36 
Running compressible is alway

#35 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
Running compressible is alway more tricky than running incompressible: there is more to go wrong. You may find that starting from the incompressible solution helps your startup problem and yes you can do this by copying the fields.
Are you running with the transonic option for the pressure? Given that your Ma is 0.7 you might find it helpful for stability. You might also find it useful to start with a very small time step and crank it up as the solution progresses. 

May 27, 2005, 15:07 
Hi Weller
Tank very much fo

#36 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hi Weller
Tank very much for your help and advises. Your answer has grown some doubts in my mind such as: "How running with the transonic option for the pressure?". How is it turned on (or setup)? I already try to begin the calculation with small time step. In fact, I use variable time set option and I impose Courant number between 0.15 and 0.3. The copy of the incompressible solution field to compressible one is donne only using "cp" OS command directly, i.e., there are not a foam utility that do it, is it? I already had success in the calculations of incompressible flow over this geometry (Airfoil). The air speed was set 10 m/s and the cord is 1 m long. I calculated using kep model and the boundary layer does not appear. The mesh is fine enough near the wall boundaries ( I hope!). Now I'm trying to guest what does not appear the boundary layer in such case! Many tanks for your help! Wladimyr 

May 28, 2005, 05:41 
transonic is an option in the

#37 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
transonic is an option in the PISO dictionary of fvSolution.
Why do you need an OpenFOAM utility reproducing the functionality of cp? If you like you could create an alias to change it's name or wrap it with a more complex alias or script if you would like to make it do more than the raw cp, it all depends on what you want from it. What patch type have you given the airfoil? What boundary conditions have you specified for p, U, k and epsilon? 

May 28, 2005, 16:23 
Hi Weller
Tank vary much fo

#38 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hi Weller
Tank vary much for your prompt answer. Excuse for my stupid questions! I have looked for some explicity transonic option in the PISO dictionary without success. And I nothing have found in the User's and Programmer's manual. Thus, is the fluxGradp switch that one for transonic flow? I haven't deep knowledge in the pressure corection methods such as PISO and SIMPLE. I come from the compressible density coupled methods schools! About patch in the airfoil, it is defined as wall and the velocity is imposed equal to zero in the U field dictionary. All anothers are left with their default values. Tank you very much again! 

May 28, 2005, 17:02 
The option is transSonic, set

#39 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 13 
The option is transSonic, set it to yes:
transSonic yes; You will also have to set the pressure solver type to BICCG rather than ICCG because the pressure matrix will become assymetric. You may also have to make some changed in fvSchemes but the code will tell you what entries are required. 

May 29, 2005, 21:57 
Hi Weller
Tank very much fo

#40 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 8 
Hi Weller
Tank very much for your prompt answer and right advise. I had success in the airfoil simulations using your advise and correcting some mistakes in the boundary conditions definitions. I have two simmetry planes which I have defined in not right way as empty. Additionally, I have acquired experience in the incompressible test case about wall BC. The better way is initialise the calculation up some converge using wall after swap it for wall function BC. For transonic case, using rhoTurbFoam, I did sucess using adiabatic wall BC and late swaping to wall function BC after some convergence is achieved. In transonic case, I did use your sugesttion: switch on the transonic flag; However, the FoamX does not acept this variable and erases it in the solution dict. when we save the case in this GUI. The same problem happens in the solution dict. when we replaces BICCG in the rho and p solvers. How and where can us modify the sources such that this problem can be solved? I started the calculations of transonic flow with uniform distribution of the properties and Courant Num = 0.3 without problem! I did not need to begin with calculations from incompressible solution. Of coarse, I spent more time to find the final solution ; You did commented something about fvSchemes needs be changed. Can you guide me where can I find the informations to do it? Tank again and in advance for your help and advises! Wladimyr 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Compressible Turbulent Flow  CFDtoy  Main CFD Forum  5  January 19, 2005 05:41 
bench mark for subsonic compressible turbulent fl  javadi  Main CFD Forum  0  June 14, 2004 08:40 
need tubulence compressible subsonic benchmark  javadi  Main CFD Forum  1  June 14, 2004 08:36 
compressible subsonic flow  Joel  CDadapco  2  April 24, 2003 08:18 
Compressible turbulent flow  FVS  Main CFD Forum  0  April 13, 2002 17:07 