[Mike_star]

Hello everyone,

I am simulating airflow in a room with a block heater using a CFD code.
Does anyone know how to implement heat flux B.C of the block heater in a finite difference CFD code? In energy equation (I mean temperature transport equation), temperature B.C. can be easily applied to the code however applying heat flux B.C. is a little tricky. Can I use T(i)=q''/h+T(i-1) to implement the boundary condition in the fluid domain (T(i) is the temperature on the surface of the heater and shall be computed, T(i-1) is the temperature of adjacent node within the fluid)? If yes, how can I determine the h coefficient?
Any help or comment is appropriated.

Mike

[FMDenaro]

Originally Posted by Mike_star

Hello everyone,

I am simulating airflow in a room with a block heater using a CFD code.
Does anyone know how to implement heat flux B.C of the block heater in a finite difference CFD code? In energy equation (I mean temperature transport equation), temperature B.C. can be easily applied to the code however applying heat flux B.C. is a little tricky. Can I use T(i)=q''/h+T(i-1) to implement the boundary condition in the fluid domain (T(i) is the temperature on the surface of the heater and shall be computed, T(i-1) is the temperature of adjacent node within the fluid)? If yes, how can I determine the h coefficient?
Any help or comment is appropriated.

Mike

On a boundary (for example a wall) you set the continuity between the conduction in the solid (flux q) and the heat flux in the fluid (-k Grad T) along the normal to the boundary. That is


-k dT/dn = q


you see that q must be known from the physics of your problem and k is known from the fluid. Then, you have to discretize dT/dn using an asymmetric FD formula (I strongly suggest to use at least a second order formula) that gives the T at the wall as a function of the internal layer and the condition q.

[Mike_star]

Originally Posted by FMDenaro

On a boundary (for example a wall) you set the continuity between the conduction in the solid (flux q) and the heat flux in the fluid (-k Grad T) along the normal to the boundary. That is


-k dT/dn = q


you see that q must be known from the physics of your problem and k is known from the fluid. Then, you have to discretize dT/dn using an asymmetric FD formula (I strongly suggest to use at least a second order formula) that gives the T at the wall as a function of the internal layer and the condition q.

Thank you for your reply. I think -k dT/dn = q equation is only applicable in solid domain where the heat conduction is dominant. However, this equation cannot be used for the fluid domain where both convection and conduction exist.
As I mentioned for obtaining the wall temperature, q=h(delta T) equation can be used. However the convection heat transfer coefficient (h) is unknown and that's my problem.

[FMDenaro]

Originally Posted by Mike_star

Thank you for your reply. I think -k dT/dn = q equation is only applicable in solid domain where the heat conduction is dominant. However, this equation cannot be used for the fluid domain where both convection and conduction exist.
As I mentioned for obtaining the wall temperature, q=h(delta T) equation can be used. However the convection heat transfer coefficient (h) is unknown and that's my problem.

No, that depends on the problem you are considering. If you are studying a CHT problem then yes, the temperature field in fluid and solid must be solved together.

Conversely, in a classical heat transfer study the heat flux q applied at a wall is a known condition, that is you do not need at all to prescribe h but only the flux. This is a classical non homogenous Neumann condition that is expressed only in terms of the normal derivative of the temperature on the boundary.

[pcosta]

Originally Posted by Mike_star

Hello everyone,

I am simulating airflow in a room with a block heater using a CFD code.
Does anyone know how to implement heat flux B.C of the block heater in a finite difference CFD code? In energy equation (I mean temperature transport equation), temperature B.C. can be easily applied to the code however applying heat flux B.C. is a little tricky. Can I use T(i)=q''/h+T(i-1) to implement the boundary condition in the fluid domain (T(i) is the temperature on the surface of the heater and shall be computed, T(i-1) is the temperature of adjacent node within the fluid)? If yes, how can I determine the h coefficient?
Any help or comment is appropriated.

Mike

Hi,

Since you are doing CFD, it doesn't make sense to lump convective effects into a heat transfer coefficient h. You are already resolving convective effects from 'first-principles' in the CFD code, since you solve for a velocity field!

So, for instance, if you use central finite differences, at the boundary i=0 you could have something like: (T(1)-t(0))/dx = q'' -> T(0) = q''dx+T(1). But this BC is not centered at the boundary, so it may be nicer to use second-order one-sided differences as suggested above, and you have for constant grid spacing:T(0) = (-2*q''dx+4*T(1)-T(2))/3 [google is your friend for confirming this result ].

I hope this helps!