CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

wallHeatTransferCoeff in chtMultiRefionFoam OF6 not working

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 18, 2018, 11:09
Default wallHeatTransferCoeff in chtMultiRefionFoam OF6 not working
  #1
Senior Member
 
Muhammad Waqas
Join Date: Jul 2014
Location: Germany
Posts: 122
Rep Power: 12
mwaqas is on a distinguished road
Send a message via Skype™ to mwaqas
Hello Everyone,

In chtMultiRegionFoam, I want to calculate heat transfer coefficient. OpenFOAM has introduced "wallHeatTransferCoeff" function object in OF6 to calculate heat transfer coefficient directly. Here is the link

I am trying to test this function. Hence, I have only included following function in controlDict to calculate the wall heat transfer coefficient.
Quote:
functions
{
wallHeatTransferCoeff1
{
type wallHeatTransferCoeff;
libs ("libfieldFunctionObjects.so");
region bottomWater;
rho 1.225;
Cp 1005;
Prl 0.707;
Prt 0.9;
}
}

But I am getting following error
Quote:
[0] --> FOAM FATAL ERROR:
[0] Unable to find incompressible turbulence model in the database[1]
[1]
[1] --> FOAM FATAL ERROR:
[1] Unable to find incompressible turbulence model in the database
[1]
[1] From function virtual bool Foam::functionObjects::wallHeatTransferCoeff::exec ute()
[1] in file wallHeatTransferCoeff/wallHeatTransferCoeff.C at line 227.

It seems like wallHeatTransferCoeff has not been for chtMultiRegionFoam, but realease note of OF6 specially mentions that it could be used to calculate heat transfer coefficient in multi-regio simulation.
Did anyone try this function? Am I missing something or making a mistake?
I took OF6 multiRegionHeater tutorial, I didn't change anything in tutorial at all

Thank you

Regards
mwaqas is offline   Reply With Quote

Old   September 19, 2018, 03:50
Default
  #2
Senior Member
 
Join Date: Sep 2013
Posts: 353
Rep Power: 21
Bloerb will become famous soon enough
This was made for incompressible solvers. Hence your error message. While chtMultiRegion can calculate incompressible flow it is still a compressible solver (which allows the user to set a constant density). If you follow the link you gave to the commit you can read

Code:
wallHeatTransferCoeff: New functionObject to calculate the wall heat …

…transfer coefficient

for incompressible flow simulated using simpleFoam, pimpleFoam or pisoFoam.
Now these solvers can be used with a -region option, but are not conjugate solvers.

This function object calculates this in the following fashion:

Code:
            wallHeatTransferCoeffBf[patchi] =
                rho_*Cp_*(nuBf[patchi]/Prl_ + nutBf[patchi]/Prt_);
It should be easy to calculate this in ParaView or via your own (coded) function object for compressible flow
Bloerb is offline   Reply With Quote

Old   September 19, 2018, 06:21
Default
  #3
Senior Member
 
Muhammad Waqas
Join Date: Jul 2014
Location: Germany
Posts: 122
Rep Power: 12
mwaqas is on a distinguished road
Send a message via Skype™ to mwaqas
Hi Bloerb,

Thank you for your reply.
Quote:
wallHeatTransferCoeff: New functionObject to calculate the wall heat transfer coefficientfor incompressible flow

You are absolutely right, it is mentioned over there that it is for incompressible flow but I couldn't find that it is only for flow using using simple. pimple or pisoFoam.
What I could find is:
Quote:
Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ];

It is meant for multiRegion (off course incompressible) and as per my understanding from this link, there is only one solver for multiregion in OF-6 i.e. chtMulriRegionFoam (they have combined both chtMulriRegionSimpleFoam and chtMulriRegionFoam in one solver i.e chtMulriRegionFoam) and chtMulriRegionFoam is by default for compressible fluid.
Quote:
Solvers: chtMultiRegionFoam conjugate heat transfer (CHT) solver runs both steady-state and transient solutions (deprecating chtMultiRegionSimpleFoam) [ commit 283f8b ]; added option for reactions and combustion to chtMultiRegionFoam [ commit 7c237a ].

Then how could we use wallHeatTransferCoeff for multi-region?

Regards
mwaqas is offline   Reply With Quote

Old   September 19, 2018, 09:54
Default
  #4
Senior Member
 
Join Date: Sep 2013
Posts: 353
Rep Power: 21
Bloerb will become famous soon enough
As I said, you can't use it with this solver without programming your own utility
Bloerb is offline   Reply With Quote

Old   September 17, 2020, 13:17
Default
  #5
Member
 
giovanni
Join Date: Sep 2017
Posts: 50
Rep Power: 9
gian93 is on a distinguished road
Quote:
Originally Posted by Bloerb View Post
This was made for incompressible solvers. Hence your error message. While chtMultiRegion can calculate incompressible flow it is still a compressible solver (which allows the user to set a constant density). If you follow the link you gave to the commit you can read

Code:
wallHeatTransferCoeff: New functionObject to calculate the wall heat …

…transfer coefficient

for incompressible flow simulated using simpleFoam, pimpleFoam or pisoFoam.
Now these solvers can be used with a -region option, but are not conjugate solvers.

This function object calculates this in the following fashion:

Code:
            wallHeatTransferCoeffBf[patchi] =
                rho_*Cp_*(nuBf[patchi]/Prl_ + nutBf[patchi]/Prt_);
It should be easy to calculate this in ParaView or via your own (coded) function object for compressible flow

Could someone explain the formula used for heat transfer coefficient mentioned above? I want to use it for an incompressioble simulation with water trough pipes . Water is at 100C and the solver used is simpleFoam. I want to visualize the "virtual" heat transfer coefficient at walls . I think that I have set correctly the function object in the controlDict :
Code:
wallHeatTransferCoeff1
    {
        type        wallHeatTransferCoeff;
        libs        ("libfieldFunctionObjects.so");
        //region      fluid;
        //patches     (".*Wall");
        rho         997;
        Cp          4215.7;
        Prl         1.64;
        Prt         0.9;
    }
the problem is that paraFoam shows me very small heat transfer coefficient... (it should be on the order of 3*10^4 but mine are on the order of 5*10^0)..

what I have missed? thanks
gian93 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
InterFoam: Different results in OF5 and OF6 vatavuk OpenFOAM Bugs 19 January 26, 2021 18:22
findCell() in parallel: not working if location is outside the domain TobiWol OpenFOAM 0 January 10, 2018 15:33
Processor 0 not working vishwesh OpenFOAM Running, Solving & CFD 0 November 17, 2017 04:35
DPM parallel is not working but serial is working johnwinter FLUENT 1 March 27, 2012 03:01
Working directory mgonzalo FLUENT 1 November 11, 2011 11:05


All times are GMT -4. The time now is 10:00.