[abidkhan]

Hello,

I've a gas enclosed inside a container at 2bar and there is no inlet or outlet. I want to study temperature profile on different components of the container as a result of heat source inside and outside of the container. How to give this 2bar pressure to the fluid because Only boundary condition I can specify is symmetry and heat source inside the fluid. I tried setting reference pressure to 2bar but even then it shows message during the solution that no pressure is specified at any boundary condition. How can handle this case?

Best Regards,
Abid

[AtoHM]

I didn't use it so far, but there is an option to set the Relative Pressure Level in Solver Control -> Advanced Options -> Pressure Level Information.

[ghorrocks]

Are you sure this is a CFD problem? It sounds like a heat transfer thing as the fluid does not appear to be moving. Please correct me if I am wrong.

If it is just heat transfer then you can use CFX to do a thermal only model. Simply define everything as solids (including the stationary fluids) and you will have a heat transfer only model.

[Opaque]

Careful with the boundary conditions.

If your thermal model only has the heat source, I assume you have the container walls set as adiabatic, correct? If that is the case, your system is not well defined since there is no reference temperature to anchor the solution to. Perhaps the container is not perfectly insulated, and there are some heat losses and you can then use the heat transfer coefficient option. The outside temperature will become the anchor then.

[abidkhan]

Originally Posted by AtoHM

I didn't use it so far, but there is an option to set the Relative Pressure Level in Solver Control -> Advanced Options -> Pressure Level Information.

Thanks for reply, I'll look into this option.

Originally Posted by ghorrocks

Are you sure this is a CFD problem? It sounds like a heat transfer thing as the fluid does not appear to be moving. Please correct me if I am wrong.

Actually buoyancy is activated and fluid also transfer some heat to container components due to its circulation within the container. Due to this, I am using it as a fluid.

Originally Posted by Opaque

If your thermal model only has the heat source, I assume you have the container walls set as adiabatic, correct? If that is the case, your system is not well defined since there is no reference temperature to anchor the solution to. Perhaps the container is not perfectly insulated, and there are some heat losses and you can then use the heat transfer coefficient option. The outside temperature will become the anchor then.

An outer surface of the container is given a high temperature from which it is getting the heat while rest of the surfaces are defined heat transfer coefficient and temperature.

I am not clear how to define Pressure value inside the fluid domain because there there is no such boundary available and solver is giving warning as I stated in my initial post.

Best Regards
Abid

[ghorrocks]

The pressure level warning is just that, only a warning. A valid transient simulation is to define the pressure in the initial condition, but have a closed domain where the pressure can vary. If your simulation is like this then you can ignore the warning and proceed.

[abidkhan]

Originally Posted by ghorrocks

The pressure level warning is just that, only a warning. A valid transient simulation is to define the pressure in the initial condition, but have a closed domain where the pressure can vary. If your simulation is like this then you can ignore the warning and proceed.

So let's say gas is filled in the container at say 2bar amd then heating is started. Solving such case in a steady state analysis, if I give initialize the setup at 2bar (when reference pressure is set 0bar) or at 1bar (when reference pressure is set 1bar), will it be correct pressure setup for the case?

[ghorrocks]

If the gas starts at 2 bar and it a sealed, rigid container then the pressure will increase. CFX can model this, and in fact it is a good test case to use as there are analytical solutions to compare to and you can see what mesh, time step and convergence you need for accurate results.

You always set the reference pressure to a typical pressure in the simulation. So if it starts at 2 bar absolute and will get to about 4 bar absolute then a reference pressure of 3 bar would be appropriate (but setting the reference pressure to anywhere between 2 and 4 bar should be fine).

[abidkhan]

Originally Posted by ghorrocks

If the gas starts at 2 bar and it a sealed, rigid container then the pressure will increase. CFX can model this, and in fact it is a good test case to use as there are analytical solutions to compare to and you can see what mesh, time step and convergence you need for accurate results.

So kind of you you for detailed reply. And yes, had starts at 2 bar and then container is sealed. No inlet. No outlet. So in this case just initializing it at 2bar would simulate the case correctly?

Originally Posted by ghorrocks

You always set the reference pressure to a typical pressure in the simulation. So if it starts at 2 bar absolute and will get to about 4 bar absolute then a reference pressure of 3 bar would be appropriate (but setting the reference pressure to anywhere between 2 and 4 bar should be fine).

So if reference pressure is set to 3bar, what would initial pressure in initialization setup? Will it be 2bar or -1bar (to count for reference pressure)?

[ghorrocks]

All pressures (well, almost all) are relative to the reference pressure. So if your device starts at 2 bar absolute and goes to 4 bar, then set the reference pressure at 3 bar and the initial pressure as -1 bar.

[abidkhan]

Thank you very much for replies.