[shiromaniac]

Hello Everyone!
I am new to OpenFOAM and I am currently working on chtmultiregionSimpleFoam and chtmultiregionfoam. Both the solvers mentioned are meant for compressible fluids but I need to run these solvers for incompressible fluids. What should I do? Does anyone have done this before( I bet many of you must have)? Please Help!

[pete20r2]

Hi Shiromani, the last time I set up a case like this I recompiled the solver to use heThermo instead of psiThermo. Then you can use the const settings in thermophysicalProperties or polynomial functions if you wish.

[Bloerb]

simply run them with incompressible settings inside thermoPhysicalProperties (rho=const) and you are good.

[shiromaniac]

Hey Bloerb,
Happy New Year and Thank you so much! It is of great help. Could you please also tell me if I want to do Forced Convection Conjugate heat transfer what should I do?? Thanks in advance!

[Bloerb]

Well heat transfer can happen by natural and forced convection inside a liquid. Lets look at how this effects the motion of the fluid:



Natural Convection

• Happens due to temperature depended density differences and gravity
• Hence enters the momentum balance via rho and f
• Temperature changes the fluid flow

Forced convection

• Happens due to pressure gradients
• Temperature does not change the fluid flow since the pressure gradient is not caused by a temperature difference but e.g a pump.

Since you have already set the density to constant and hence incompressible flow you have already eliminated free convection. This is also why all heat transfer solvers are compressible inside OF. If you are solving incompressible flow, heat transfer and fluid flow are not coupled. This means fluid flow will be the same with or without heat transfer (assuming that your liquids properties are not temperature depended e.g temperature depended viscosity).

Hence you can use the chtMultiRegion class of solvers for forced and natural convection. You "simply" need to create your mesh and choose the right boundary conditions.

[Raza Javed]

Originally Posted by Bloerb

Well heat transfer can happen by natural and forced convection inside a liquid. Lets look at how this effects the motion of the fluid:



Natural Convection

• Happens due to temperature depended density differences and gravity
• Hence enters the momentum balance via rho and f
• Temperature changes the fluid flow

Forced convection

• Happens due to pressure gradients
• Temperature does not change the fluid flow since the pressure gradient is not caused by a temperature difference but e.g a pump.

Since you have already set the density to constant and hence incompressible flow you have already eliminated free convection. This is also why all heat transfer solvers are compressible inside OF. If you are solving incompressible flow, heat transfer and fluid flow are not coupled. This means fluid flow will be the same with or without heat transfer (assuming that your liquids properties are not temperature depended e.g temperature depended viscosity).

Hence you can use the chtMultiRegion class of solvers for forced and natural convection. You "simply" need to create your mesh and choose the right boundary conditions.

Hi,


Your answer is very helpful for my case also. because I am also stuck in incompressible and compressible thing.


I have heat transfer and fluid flow also. The walls of the fluid region are hot and fluid is flowing from inlet and outlet. and it must take this heat out at the outlet.


So, in this case, if I set (rho = constant) in constant/fluid/thermophysicalProperties, it means that my flow is incompressible NOW, and there is no coupling between fluid flow and heat transfer?


And in case I want to simulate compressible flow, then what should I write for "rho" in themophysicalProperties?


I shall be very thankful if you can clear my doubts.


Thank you

[Bloerb]

Yes, if rho is set to constant your flow solution does not depend on temperature. If you want to simulate something compressible you need to switch from rhoConst to e.g perfectGas or one of the many other possibilities:

https://cfd.direct/openfoam/user-gui...hermophysical/

[Raza Javed]

Originally Posted by Bloerb

Yes, if rho is set to constant your flow solution does not depend on temperature. If you want to simulate something compressible you need to switch from rhoConst to e.g perfectGas or one of the many other possibilities:

https://cfd.direct/openfoam/user-gui...hermophysical/

Thank you so much for your help.


I have one question here, when I set these options, then how to decide the rhomax and rhomin in the system/fluid/fvSolutions file?



because before I was using (rho = 1000) in constant/thermophysicalProperties, so I set the rhomax and rhomin = 1000, but now I changed the rho from constant to icoPolynomial.

[Bloerb]

Well you need to set a maximal and a minimal value that could occour in your simulation.
For example 0 and 10000000000000 would suffice. Setting closer ranges might make it more stable during start up

For water with rho from 900 to 1100 e.g 700 and 2000 for stability

[Raza Javed]

Originally Posted by Bloerb

Well you need to set a maximal and a minimal value that could occour in your simulation.
For example 0 and 10000000000000 would suffice. Setting closer ranges might make it more stable during start up

For water with rho from 900 to 1100 e.g 700 and 2000 for stability

Hi.


Thank you so much. It was very helpful.


Thank you once again.


Regards


Raza

[Raza Javed]

Originally Posted by Bloerb

Well you need to set a maximal and a minimal value that could occour in your simulation.
For example 0 and 10000000000000 would suffice. Setting closer ranges might make it more stable during start up

For water with rho from 900 to 1100 e.g 700 and 2000 for stability

Hi,


I have one question relating to relaxation factor.


1. What is relaxation factor and what is under relaxation?

2. How can we decide that what value of relaxation factor do we need?
3. what is the upper and lower limit of relaxation parameter? OR we can put any value?
4. In my simulation, when I reduced the relaxation factor to a very very lower value then my residuals goes to minimum value very fast.



But I couldn't exactly get, that how relaxation factor affecting my simulation and how can I change it to get the desired results.


I shall be thankful for your help.


Thank you

[Bloerb]

If you do not know what a relaxation factor is, you should not do numerical simulations. That is the harsh truth. The more modest response would be to not touch them, since the standard values are fine. And in this case it is not to much to ask to google it and read a wikipedia article.

[Owais Shabbir]

Originally Posted by Raza Javed

Hi,


I have one question relating to relaxation factor.


1. What is relaxation factor and what is under relaxation?

2. How can we decide that what value of relaxation factor do we need?
3. what is the upper and lower limit of relaxation parameter? OR we can put any value?
4. In my simulation, when I reduced the relaxation factor to a very very lower value then my residuals goes to minimum value very fast.



But I couldn't exactly get, that how relaxation factor affecting my simulation and how can I change it to get the desired results.


I shall be thankful for your help.


Thank you

Hi,
I will try to give basic explaination. And Bloerb is right you should invest sometime in learning the basic about convergence, residuals and underrelaxation (U).

residual_new = residual_old + U (residual_new_predicted - residual_old)

So underrelaxation factors are basically to supress the oscillation in the flow solution. These osciallation are a result of numerical errors.

Smaller the underrelaxation means, for sake of the simplicity lets say, allowed to much of 'acceptance' to have errors in your solution. The residuals will start to converge and you might think the solution is converged when in reality it is not.

Recommended is to use as high as possible. But note high underrelaxation lead to oscillation in the solution so that's why as high as possible so you don't have oscillations. If you are studying the tutorials and do not wish to learn about the convergence rate, I'd say they are already good.

U < 1 means underrelaxation. Slows down speed of convergence but increases stability (Hence in your case residuals reach low value)
U=1 means no relation. Good for predicting values of the variable
U>1 means over relaxation. Good if you want to accelerate your convergence but decreases the stability

Hope this helps.
OS

[ardim]

Originally Posted by Bloerb

[...]
Since you have already set the density to constant and hence incompressible flow you have already eliminated free convection.
[...]

Well, that’s not true if you are modeling natural convection in incompressible air with the Boussinesq approximation. I’ve opened a new thread, asking for examples, here: Example or tutorial suitable for this buoyancy coupled problem?

Does this mean there’s no solver in OpenFoam for solving a model like the one in that thread? (actually the conjugate heat transfer could be very simple in my model: radiation from walls to other walls could be ignored, and the temperature in the contiguous rooms can be assumed a constant value).

Thank you very much for any help you could provide!!