[Thomas Baumann]

Hallo Foamers,

I'm simulating channel and pipe flows using LES with forced convection and heat transfer. I have modified pisoFoam to solve four temperature-equations for four different molecular Prandtl numbers. As wall boundary condition I'm using a fixed gradient. So the medium is getting warmer over the time.

For cycling the velocity I'm using the directMapped bc. But I don't want that my temperature is growing in the inlet and so I have implemented a boundary condition that solves that without using directMapped:
T_inlet = T_outlet- deltaT. And deltaT is a fixed value that I have determined. This one works but I have problems using many processors. So I'm trying to program a new directMappedbc where I can use deltaValue instead of average.

I made a new bc with the name moddirectMappedFixedValue and compiled dynamically the origin directMapped using wmake libso as discribed in the wiki. It works, I can select it as boundary condition, but when I'm solving an easy validation case I get following error:


Create mesh for time = 0

Reading field T1

pisoTempFoam: symbol lookup error: /user/hi204/OpenFOAM/hi204-1.7.0/lib/linux64GccDPOpt/libmoddirectMappedFixedValueFvPatchField.so: undefined symbol: _ZN4Foam37moddirectMappedFixedValueFvPatchFieldIdE C1ERKNS_7fvPatchERKNS_16DimensionedFieldIdNS_7volM eshEEERKNS_10dictionaryE


I'm not an expert of C++. So it would be very kind if someone could help me.

Best regards, Thomas

[harishg]

Did you compile it in user folder or within the original boundary condition folder? If you did the former, you need to add

libs("whatevername.so") to your system/controldict

[Thomas Baumann]

Thank you very much for the answer.

I compiled it dynamically. So I had to include libs("whatevername.so") to your system/controldict

So when I'm solving the test case I don't get the error that the new boundary type can't be found, it's an error while using the new boundary type.

Here you can download the code for the boundary-condition
http://www-isl.mach.uni-karlsruhe.de/~hi204/OpenFoam_Forum/newbc

Regards, Thomas

[harishg]

For some reason the linker is not able to look up for the BC while running the solver. You can try recompiling OpenFOAM by running wclean and wmake. Another temporary fix is to copy the boundary conditions files into your solver folder and recompile the solver: http://www.tfd.chalmers.se/~hani/kur...yCondition.pdf

and see if it works for now.

[Thomas Baumann]

Hi,

thanks again. But that was not the problem. But I solved it now.
I had to include in the moddirectMappedFixedValueFvPatchField.H data:

#ifdef NoRepository
# include "moddirectMappedFixedValueFvPatchField.C"
#endif

and change that
moddirectMappedFixedValueFvPatchField.C is not included in the files data.

Than I changed
setAverage_ to setHeating_

and

average_ to heating_

and I changed in the moddirectMappedFixedValueFvPatchField.C:
if (setHeating_)
{
Type heatingPsi =
gSum(this->patch().magSf()*newValues)
/gSum(this->patch().magSf());
newValues += heating_;
/*if (mag(heatingPsi)/mag(heating_) > 0.5)
{
newValues *= mag(heating_)/mag(heatingPsi);
}
else
{
newValues += (heating_ - heatingPsi);
}*/
}


and changed in the moddirectMappedFixedValueFvPatchField.H
TypeName("moddirectMapped");


now I can use for example:
inletpatch
{
value uniform 300;
type moddirectMapped;
setHeating on;
heating -176.249998;
}

and it works without any problems until now

Regards Thomas

[David_010]

Hi Thomas,

First of all tanks for your attention. I have been using the directMapped b.c for the temperature field, with a fixed heat flux at the wall of a duct. In my case, I need to have the same average temperature at the inlet, because if I use a fixed gradient b.c at the wall, I don't know the temperature difference between inlet and outlet at the beginning. So, I impose an average value for the temperature at the inlet, while the temperature profile is the same as at the outlet.


My question is, how can you impose a temperature step between inlet and outlet or, how do you know it?


I have another question. In my problem, laminar flow in a duct with moving devices inside, I get correct results for low Prandtl numbers (e.g air) but the temperature increases a lot and the results are wrong when I tray to solve for high Prandtl numbers (e.g 280). I have thought about numerical diffusion, but may by you know what could be the problem.


Thank you again for your help.


Regards,


David

[Thomas Baumann]

Hi David,

I made a energy-sumation. Thermal Energy which comes in due to the inlet + thermal energy due to the wall heat flux = thermal energy out due to the outlet. So it's only heat balance. Because of I'm simulating a incompressible flow and the viscosity and the molecular Prandtl number etc. are constant I can determine at the beginning the DeltaT value, which the medium will be heated passing the flow regime.

For your other question I don't undersand it. I need more details. What bc's do you use, incompressible, which solver, turbulent..

Best regards

Thomas

[David_010]

Hi Thomas,

Thanks a lot for your reply. I've looking for a boundary condition like yours for a long time. I am working in a model of heat exchanger which is a tube (with constant heat flux at the walls) with moving scrapers inside, in order to increase the heat transfer. So, I want to simulate only one pitch of the heat exchanger, and I am using the directMapped b.c for velocity, but I need a b.c like yours for the temperature. How do yo specify the initial temperature at the inlet, or the initial temperature?


My second question was: I have validated the model of the heat exchanger, employing an incompressible, steady and laminar solver (basically buoyantBoussinesqSimpleFoam) for low Prandtl numbers (e.g air properties Pr=0,7). The velocity and temperature profiles are exactly like the analytical ones, and the energy balance is also accomplished. But when I change the properties to a high Prandlt number (e.g propylene glycol Pr=280) the temperature increases to values higher than expected, and the energy balance is not accomplished, with errors about the 80%.


The boundary condition I'm using is a fixedGradient b.c for the temperature at the wall, inlet is uniform with T=300K, and outlet is zeroGradient.


I have thought about a problem of numerical or false diffusion, but the problem continues if I change the numerical scheme (blended, Gamma...).


Thank you very much again for your help, at this point I am a bit lost.


Regards


David

[Thomas Baumann]

Hi David,

I was using as starting condition a constant temperature over the complete field. After a while the temperature field will be developed , too. I can do that, because I use the assumptions that the flow is incompressible and nu Pr ... are constant. With the new bc condition I can cycle the temperature, too. To determine delta T, which I have to add or remove I made a heat balance as descirbed above.

If you have flows with high Prandtl numbers you can get turbulence on the heat side. The critical number is hereby the Peclet number. (Peclet number = molecular Prandtl number* Re)
So here your velocity is due to the diffusivity laminar, but your thermal diffusivity is too low and so you get an thermal instability...
Maybe that could be the problem.

Send me your email adress and I will send zou the code.

Best regards

Thomas

[grandgo]

Originally Posted by Thomas Baumann

Hi David,

I was using any starting condition a constant temperature. I can do that, because the flow is incompressible and nu Pr ... are constant. With the new bc condition I can cylcle the temperature , too. To determine delta T, which I have to add or remove I made a heat balance as descirbed above.

If you have flows with high Prandtl numbers you can get turbulence on the heat side. (Peclet number = molecular Prandtl number* Re)
So here your velocity is due to the diffusivity laminar, but your thermal diffusivity is to low and so you get an thermal instability...
Maybe that could be the problem.

Send me your email adress and I will send zou the code.

Best regards

Thomas

hi thomas,

could you please send me the code of your modified pisoFoam solver? it sounds very interesting to me.

which turbulenceModel are you using?

best regards
grandgo