|
[Sponsors] |
wallHeatFlux utility for an incompressible case |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 19, 2013, 09:48 |
|
#21 |
New Member
ae-lab VUB
Join Date: Oct 2011
Posts: 17
Rep Power: 14 |
hi
Is there a example/tutorial on how to use the wallHeatFluxIncompe utility? What should be included in the wallHeatFluxDict? Thx! |
|
December 29, 2013, 16:43 |
|
#22 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Greetings aevub,
Well... I had already mentioned in my previous post where a "wallHeatFluxDict" can be found: Quote:
This is because the one mentioned on the quoted post is for a modified version of the one in #12. As for an example case... my guess is that you can use any tutorial case that uses heat transfer and uses incompressible flow. Best regards, Bruno
__________________
|
||
May 19, 2014, 08:03 |
|
#23 |
New Member
Chris
Join Date: May 2014
Posts: 2
Rep Power: 0 |
Hello,
i have an other problem with using the wallHeatFluxIncompressible tool. I'm computing a case with the buoyantBoussinesqPimpleFoam in OF 2.2 with k-w SST and wall-functions. When i'm using the tool it makes the error: --> FOAM FATAL IO ERROR: Unknown patchField type kappatJayatillekeWallFunction for patch type wall Valid patchField types are : ... Sure i can change the wall function and recompute it but is there a solution with this wall-function? thanks |
|
June 22, 2014, 15:08 |
|
#24 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
I've created a git repo for the utility wallHeatFluxIncompressible by Eelco van Vliet: https://github.com/wyldckat/wallHeatFluxIncompressible In addition, I've adapted the code to work with OpenFOAM 2.2.x and 2.3.x. Note: When using OpenFOAM 2.2.0, you should use the code that is meant for OpenFOAM 2.1.x, because the field names in 2.2.0 are still using the old field naming convention "kappat" and "kappaEff", while 2.2.1 and above use "alphat" and "alphaEff". @Chris: I don't know if you've managed to solve the problem you had, but if you're using OpenFOAM 2.2.1 or 2.2.2 or 2.2.x, then try using the code from the repository I've indicated above. Best regards, Bruno
__________________
|
|
October 30, 2014, 06:49 |
|
#25 | |
New Member
Kostas Margaris
Join Date: Feb 2014
Posts: 15
Rep Power: 12 |
Hi all!
I have created a simple model (attached) of natural convection inside a rectangular domain. I used the wallHeatFluxIncompressible utility to check the heat flux balance. I got the expected result, 10 W/m2 were applied to wall4 as BC and 10 W/m2 are coming out wall3 which had a constant temperature BC: Quote:
Could someone explain why this is happenning? |
||
October 30, 2014, 07:00 |
|
#26 | |
Senior Member
anonymous
Join Date: Aug 2014
Posts: 205
Rep Power: 13 |
Quote:
Code:
surfaceScalarField heatFlux =fvc::interpolate(kappaEff*Cp0*rho0)*gradT; This is the only thing I can imagine that can explain it, but I'm pretty sure I'm not right. |
||
November 1, 2014, 16:35 |
|
#27 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
@kmargaris: From the files in the case you provided, I had to guess that you used the solver buoyantBoussinesqPimpleFoam. The answer by ssss seems to be correct. More details:
Essentially, the inverted equation implemented in the boundary condition would be this: Code:
q_ = gradient()*(Cp0*alphaEffp) I took a quick look at the compressible implementation of this boundary condition... and it's essentially the same equation, i.e.: Code:
q_/(alphaEff*thermo.Cp)
So, essentially, the problem is that the heat flux used in the boundary condition is actually "q/rho", i.e. the possibly named kinematic heat flux... Mmm... I'll report this on the bug tracker... edit: Bug reported at http://www.openfoam.org/mantisbt/view.php?id=1433 Best regards, Bruno
__________________
Last edited by wyldckat; November 1, 2014 at 17:19. Reason: see "edit:" |
|
November 3, 2014, 04:56 |
|
#28 |
New Member
Kostas Margaris
Join Date: Feb 2014
Posts: 15
Rep Power: 12 |
@wyldckat: Thanks for the explanation and for submitting the bug report.
It seems that this bug only affects the post processing; the actual heat flux boundary condition is applied correctly in this case, right? |
|
November 8, 2014, 09:20 |
|
#29 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Hi kmargaris,
The boundary condition is incorrect. It would only be correct if Cp0 value was in fact "Cp*rho". In other words, you can fix the problem for the boundary condition if you simply define "rho" as 1.0 and that "Cp0" is the result of "Cp*rho". Best regards, Bruno
__________________
|
|
January 7, 2015, 01:26 |
Dear wyldckat
|
#30 |
New Member
Seokwon Whang
Join Date: May 2012
Posts: 25
Rep Power: 14 |
@ wyldckat
hello, I tried to use your 'wallHeatFluxIncompressible' in my problem. (buoyantBoussinesqPimpleFoam with LES, oneEqEddy) (I think my result is reasonable when I comparing the temperature and velocity with literature.) Your utility was completely working and calculating wallHeatFlux! When I plot the wallHeatFlux, the trend is similar with literature, however, the magnitude is totally different. (e.g. literature: 100, my case: 0.1) Do you have any idea for this problem? I use Cp0 =1.005, rho0=1.166 Thank you |
|
January 11, 2015, 15:35 |
|
#31 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Greetings hswzzz,
I'm sorry to say that you haven't provided enough information in order to deduce what might be wrong. Nonetheless, if I have to guess, since the discrepancy is at a scale of 1000, then my guess is that you were not careful enough with the units of the final mesh. OpenFOAM deals with metre by default and you probably planned for the mesh to be in millimetre. Best regards, Bruno |
|
March 16, 2015, 12:54 |
|
#32 |
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Hi Foamers,
Sorry for restarting the thread again.i am using buoyant boussinesq simpleFoam. i have read most of the threads here how to calculate wall heat flux. now i got a question may be its dumb, I have given temprature b.c on a surface patch is it now possible to find the heat flux on this patch after the simulaion? i tired the wallheatflux command on the terminal. can somebody help me. Thank You. regards, Naresh |
|
March 16, 2015, 15:24 |
|
#33 |
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Hi Bruno,
I also used the turbulentHeatFluxtemperature to specify the heat flux boundary conditions for a patch and i got unphysical result. i m using buoyantboussinesqsimpleFoam. Now i understand the reason. Thanks for the explanation. That being said is there any other posibility to specify heatFlux boundary condition for a patch? 2. i have another doubt could you please through some light on why should Cp0 should be specified as 1.0. because for TurbulenceHeatFluxTemperature B.C Cp0 is specified as 1006 though they both has the same dimensions m^2/s^2/k This is very crucial for me right now . thank you. regards, Naresh Yathuru Last edited by Naresh yathuru; March 17, 2015 at 12:43. |
|
April 5, 2015, 08:04 |
|
#34 | ||
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Greetings Naresh,
Installation instructions for compiling wallHeatFluxIncompressible are given here: https://github.com/wyldckat/wallHeatFluxIncompressible Usage instructions are given in post #19. Quote:
It's not "Cp0" that should be set to "1.0", it's "rho0" that should be "1.0", as already explained in post #29: Quote:
Best regards, Bruno
__________________
|
|||
April 7, 2015, 02:57 |
|
#35 |
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Hello bruno,
thank you so much for the reply. I have read the posts you have mentioned already. and sorry if my question was not clear. My question was concerning the wallHeatfluxIncompressible. in the readme file it says the following: Modified version of wallHeatFlux based on suggestion of to change combustion flow to normal flows http://www.cfd-online.com/Forums/ope...ance-flow.html I replaced the createField with the boussinesqSimpleFoam In this version it is required to specify values for the density, heat capacity, and Prandtl numbers in the transportProperties dictionary like Code:
// Laminar Prandtl number Pr Pr [0 0 0 0 0 0 0] 0.9; // Turbulent Prandtl number Prt Prt [0 0 0 0 0 0 0] 0.85; // Cp0 value needed for wallHeatFluxIncompressible rho0 rho0 [1 -3 0 0 0 0 0] 1.2; // this rho0 // rho0 value needed for wallHeatFluxIncompressible Cp0 Cp0 [0 2 -2 -1 0 0 0] 1.0; // i meant this cp0 may be this is a silly question could you tell me please which value should i use for cp0 and rho0 when i use turbulentwallheatFlux B.C and if i m using the wallheatfluxincompressible utility to find the flux on the patches. should i use Cp0 = 1.0 or 1005. Thank you, regards, Naresh Last edited by wyldckat; April 12, 2015 at 16:07. Reason: Added [CODE][/CODE] |
|
April 12, 2015, 16:13 |
|
#36 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,978
Blog Entries: 45
Rep Power: 128 |
Hi Naresh,
Quote:
In other words, if you don't indicate how your case was originally created and defined, I don't know how is should be handled at the end of the simulation. Best regards, Bruno |
||
April 13, 2015, 12:43 |
|
#37 | |||
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Quote:
Code:
dimensions [0 0 0 1 0 0 0]; internalField uniform 293; //17C boundaryField { inlet { type fixedValue; value uniform 293.15; // 20C } outlet { type zeroGradient; } sideandfloorwalls { type zeroGradient; } lightingwall { //type wallHeatFlux; //heatFlux uniform -200; // This did not work for incompressible flows. I read somewhere that this B:C does not exist in OF 230 type turbulentHeatFluxTemperature; heatSource flux; q uniform -200; // w/m^2 // This is just a check . this would generate a surface temperature of -27 C alphaEff alphaEff; value uniform 273; // place holder } /*{ type fixedValue; value uniform 323.15; // for the time being or flux 100 w/m }*/ innercube { type zeroGradient; //value uniform 313.15; } roof { type zeroGradient; //value uniform 291.15; } } and this how i specified my transport properties Quote:
when i use turbulentHeatFluxtemperature boundary condition i specify cp0 as 1005. but according to the read me file in the wallheatfluxincompressible it says Quote:
i m a little confused. Thank you Regards, Naresh |
||||
April 15, 2015, 05:12 |
|
#38 |
New Member
Gautam Saikia
Join Date: Jan 2015
Location: India
Posts: 12
Rep Power: 11 |
Hi Eelcovv
Can you please suggest how to use the "wallHeatFluxIncompressible" utilty file. I mean is it like just cope paste the files to the respective directory and than running the utility command from the terminal will work?? Warm regards Gautam |
|
April 15, 2015, 05:28 |
|
#39 |
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Hi goutham,
I use it this way. I copy pase the respective files eg, GradT and other required files in the 0 folder before starting the simulation. after the simulation is done u can type wallHeatfluxTemperature and the patchname in yout terminal . it is basically a post processing utility. i assume u already installed the wallHeatFluxIncompressible utility successfully and checked . All the best. Naresh |
|
April 15, 2015, 10:13 |
|
#40 |
New Member
Gautam Saikia
Join Date: Jan 2015
Location: India
Posts: 12
Rep Power: 11 |
Hi Naresh
Thanks for your reply. I just downloaded the zipfile given in this thread. After that I am not understanding if to copy the folder to "/applications/utilities" or some other steps to follow. Please help me. Thanking you Gautam |
|
Tags |
incompressible, open foam, wallheatflux |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
how to create an internal fan for a multiRegion case? | phsieh2005 | OpenFOAM | 0 | February 2, 2012 16:32 |
wallHeatFlux utility in OpenFoam1.6 | maruthamuthu_venkatraman | OpenFOAM | 29 | October 3, 2011 10:43 |
thermal analysis - how to model internal fan? | Pei-Ying Hsieh | Main CFD Forum | 6 | March 20, 2008 10:35 |
Free surface boudary conditions with SOLA-VOF | Fan | Main CFD Forum | 10 | September 9, 2006 12:24 |
flow simulation across a small fan | jane luo | Main CFD Forum | 15 | April 12, 2004 17:49 |