Accessing node value
 

Hello Sir,
In my transient analysis, at present i am calculating convection losses from a surface with the help of CEL. Where i am considering Average temperature of wall (Please refer figure). Based on which i am updating my applied boundary conditions. Is it possible to calculate convection loss for each node instead of considering Average temperature (please refer figure).

http://postimg.org/image/vhb68y2ph/

Thank you
Suneel

You do not need to, it does work as you described on the second figure.

A CEL expression is evaluated at each node; therefore, if you write an equation for q = h * (T - 25 [C]), it is evaluated at every node in the boundary as

q_node = h_node * (T_node - 25 [C]).

h_node can also be an expression; therefore, it can also be node based.

node value
 

Hello Sir,
Thank you for your quick reply. I want some clarification in this. whether we need to define it as T@WALL or (T)@WALL. I want to access temperature of particular wall to update boundary conditions.

Thank you
Suneel

Are you saying that the wall heat flux, q, at say Wall1 is a function of the temperature of another wall, say Wall2 ? I hope that is not your case since it is not trivial in any code since both walls could have different mesh topologies.

If you need q_node_wall1 = h_node * (T_node_wall1 - 25 [C])

you still do not need to specify the wall for the temperature since it is implied by context. The expression is evaluated at wall1, and all the variables used will be evaluated at wall1.

Wall out side heat flux is a function of surrounding air temperature (Ex: Ambient air) and presently not modeled. The method you suggested is works well in CFD post but Sir i want it in CFX-pre.

What you seem to be describing is a well supported boundary condition; therefore, I do not understand what you are trying to do.

What is wrong with the Heat Transfer Coefficient boundary condition already available in the software. It does exactly what you have described so far. You must specify the external heat transfer coefficient, and the external temperature and the heat flux is computed as q_node = h_node * (T_node - T_outside)

If the above is not what you need, could you please describe what you are trying to model first, then how you are trying to approach with the available functionality ? The more detailed the explanation, the easier for the forum members to help you.

Hello Sir,
At present i am calculating convection loss(Please refer figure) as follows
Q_convection = h (T_wall - T_ambient) where
T_wall_1 = areaAve(T)@Wall (Average temp of wall) and i am having ambient temperature data.
I want to calculate convection losses for each node for example
Q_convection_i = h(T_wall_i - T_ambient) where i is for different nodes on the WALL_1.

Thank you

http://s26.postimg.org/pujv8l6ih/2_question.png

Based on your description, I stand by what I said earlier. That is what the Heat Transfer Coefficient boundary condition does. No need to rewrite the implementation you already paid for. More likely, you would not get the same robustness/convergence behavior provided by the ANSYS CFX solver.

The Convection heat loss can be later recomputed in CFD-Post using

Q_convection = External Wall Heat Transfer Coefficient * (Temperature - T_ambient)

By using expressions, you do not need to know the nodes, nor loop over them either. If you still need to see the nodal distribution associated with each node, you can export a User Defined variable representing the expression above for the boundary you are interested in.