Heat in a cooling systems disappears
Hello comunity,
my overall goal is to simulate a cooling battery.
To ilustrate my problem I simplify the model to a two part model. The model shown in the picture consists of two parts (an aluminum profile, which induces heat) and a water pipe which should take the heat.
My values set for the simulation are:
-Heat source: 100.000 W/m^3 (constant)
-constant inlet velocity: 0,1m/s in normal direction with inlet temperature (298K)
-outlet: default conditions
-Wall (see picture two) are the 4 walls connecting the aluminum and the water. you see the thermal boundary condition in picture two as well (flux, heat flux 0, convective heat coefficient=2300 and heat reference temperature 298K. the alpha=2300 is a value from the internet for a water flow inside a pipe.
-default Wall (in picture 2 the brown surfaces): boundary conditions: flux, heat flux 0, convective heat coefficient 0, convective heat reference temperature 273.16K
In picutre 3 "results" you can see the temperature profile. the results kind of make sense to me, but the actual values are not matching my analytical calculation.
Using the formula Q=mass flow*c_p_water*DeltaT the output temperature should be 298.478K if Q=75.000W (Heat source W/m^3*Volume 0.75 m^3), c_p_water=4183J/kg/K and T_in=298K. The average output temperature in the simulation is 298.0477K so 1/10 of the analytical result. Same thing for my original battery simulation. The output temperature analytically calculated should be 302.5K, the result is 300K in regard to inlet temperature of 298K. So Delta T in my orignal simulation is about a factor of 2.5 away from each other.
It seems to me, that not all the heat is absorbed by the water, but dissapears anywhere. But for what I understand I have set all heat transfer at the default wall to zero, so only the water can take the heat.
I hope my problem is understandable and there is any help for me. I really have no solution as a new user for hyperworks cfd.
Kind regards
Daniel
Best Answer
-
The boundary condition for the surfaces between the fluid and solid should be as default:
heat_flux = 0, convective heat coefficient = 0 (reference temperature doesn't matter when the coefficient is zero.
This will then calculate the 'natural' heat flux between the two volumes based on material properties, temperature difference, etc. These parameters give the option of adding additional heat flux beyond that 'natural' calculation - as if you had a heat tape wrapped around, but not modeled in the mesh, etc.
The external boundary (no mesh on the other side) with heat flux = 0 and convective heat coefficient = 0 will give the 'insulated' boundary condition.
The results will depend on mesh resolution and convergence. Based on the 'result' image, I would guess the mesh is extremely coarse, and thus would not provide a solution very close to the analytical result. It could be as simple as building a finer mesh, capturing the fluid boundary layer better, good volume mesh resolution, at least three or four layers of elements in the solid, etc.
1
Altair EmployeeAnswers
-
I believe you have give convective coefficient of 2300W/mK in the water-aluminum interface. I this that's not required, in fact that should be the output for your simulation if I'm not wrong. Good Luck.
1 -
Thank you for your answer. I kind of thought the same, because the convective coefficient is a very complex value, depending on many factors. To set a constant value for that seemed wrong to me, but in many altair tutorials was this the case. They set a value for alpha to define the heat transfer between fluid and solid.
My question then is, what happens if I set alpha to 0? Because in the results I still see a heat transfer, so that means the solver is calculating heat transfer. But what value or condition do I have to set, if I want adiabatic interfaces?
0 -
Daniel_21749 said:
Thank you for your answer. I kind of thought the same, because the convective coefficient is a very complex value, depending on many factors. To set a constant value for that seemed wrong to me, but in many altair tutorials was this the case. They set a value for alpha to define the heat transfer between fluid and solid.
My question then is, what happens if I set alpha to 0? Because in the results I still see a heat transfer, so that means the solver is calculating heat transfer. But what value or condition do I have to set, if I want adiabatic interfaces?
In Hyperworks Tutorials they have specified convective coefficient for outer walls (which are exposed to ambient temperature) not on the fluid solid interface, so don't specify anything and run the case. That should convince your energy balance energy balance calculations.
0 -
The boundary condition for the surfaces between the fluid and solid should be as default:
heat_flux = 0, convective heat coefficient = 0 (reference temperature doesn't matter when the coefficient is zero.
This will then calculate the 'natural' heat flux between the two volumes based on material properties, temperature difference, etc. These parameters give the option of adding additional heat flux beyond that 'natural' calculation - as if you had a heat tape wrapped around, but not modeled in the mesh, etc.
The external boundary (no mesh on the other side) with heat flux = 0 and convective heat coefficient = 0 will give the 'insulated' boundary condition.
The results will depend on mesh resolution and convergence. Based on the 'result' image, I would guess the mesh is extremely coarse, and thus would not provide a solution very close to the analytical result. It could be as simple as building a finer mesh, capturing the fluid boundary layer better, good volume mesh resolution, at least three or four layers of elements in the solid, etc.
1