Hi, I m trying to solve laminar periodic flow (both velocity and temperature) for a wall heated channel with momentum and heat source defined on subdomain in CFX10. periodic velocity is achieved but temperature at inlet and outlet is still falling down continuously after a long run. i defined steady flow simulation and getting energy imbalance and other residuals satisfactory. can anybody please let me know why i am not getting temperature converged to a constant value while velocity has already been achieved contant at anywhere in the fluid? I defined energy source as "heat flux * area subjected* velocity u/(fluid volume* average velocity)". can u please let me know is that the correct formula for defining energy source for periodic flow?

Thanking you, Husain

Hi,

You will need to describe your simulation better for us to really help.

Some thoughts: 1) Heat can take a while to stabilise as it needs to convect around the domain. In areas of slow flow (this includes the boundary layer) this can take quite a while. Try increasing the physical time step.

2) Now you have a solution converged in velocity you could also stop the solution of the continuity and momentum equations and leave the heat equations only. This will speed things up also.

3) If your heat source is taking heat away from the fluid is something adding it so the net heat flux is zero? Obviously if their is a net heat flux into the fluid then no steady state solution exists.

Glenn Horrocks

thanks Horrocks for ur useful suggestions, the problem can be defined as: steady laminar flow in a rectangular channel with periodic boundary conditions at inlet and outlet. heat flux is defined at rest of the 4 walls of the channel. inlet and outlet are periodic in both sense temperature and velocity. Since i am using CFX-11, i did not define momentum source to maintain periodocity. CFX-11 has an option to assign mass flow on the periodic surface this is what i did. to maintain thermal periodicity i defind heat source through a subdomain as "heat flux * area subjected* velocity u/(fluid volume* average velocity)". constant velocity has been acchieved at any point in the domain within 200-300 iterations. But average temperature at periodic interfaces and at anywhere in the domain falling slightly as the simulation proceeds in time. As u said earlier, i stopped continuity and momentum equations solutions and increased physical time step for energy equation by a factor of 15. after a long run (5000 iterations) temperature does not settle to a constant value. although the temperature gradient is very small with a value of "0.5K/3.0s". whereas the timestes was 7.5e-4s after incereasing by a factor of 15 to the aotomatic timestep.

i want to know whether the expression i used for heat source is correct. if correct why did not i get temperature constant and if wrong please tell me the correct heat source expression and how can i control temperature fall? imbalance is -0.0015%.

Husain,

Hi,

In a long channel the flow velocity will eventually fully develop. This means the velocity field does not change along the length of the channel. You seem to have achieved this.

However you seem to have put a heat flux on the walls of this channel. Obviously as the fluid continues along the channel it will then heat up or cool down. There is no fully developed temperature profile of this type of flow.

If you know your model is both fully developed in both velocity and temperature then you have modelled it incorrectly. The best option to fix it would be to make one wall a constant temperature wall, or some other heat transfer relationship to a fixed temperature.

Glenn Horrocks

It seems to me that you have put a heat flux into the fluid but do not have a temperature