[sasanghomi]

Dear friends,

I am trying to simulate conjugate heat transfer. In fact, I have an excel file in which the value of heat loss is written for different positions. That is,

X Y Z HeatLoss[W]

1 0 2 20

2 6 8 50
............

....

...

How Can I import this file into Fluent (as a heat source)?

I appreciate your attention.

Best Regards
Sasan Ghomi

[AlexanderZ]

1. open your case in fluent
2. initialize the case and write heat flux profile from the surface you are interested it. You will get coordinate of each center of finite surface with respective heat flux value
3. change heat flux values in profile according to your file using interpolation (or any other method)
4. read profile, apply it as boundary condition

[sasanghomi]

Thank you for your response.
However, I want to allocate the heat loss to some regions not just some boundaries.
Do you have any idea for allocating the heat source in a 3D region?

Best Regards

[AlexanderZ]

it is same approach, choose volumetric heat source

[sasanghomi]

Thank you so much.
I have written something like below;

3
3
3
1
Volumetric Heat
(-0.0005
-0.005
-0.005
)
(0.07
0.04
0.06
)
(-0.03
0.01
0.07
)
(5000
6000
7000
)

However, I know that the name "Volumetric Heat" should be replaced by a correct name. I have no idea about the right name for the volumetric source of energy. Could you give me a hint, please?

One more question; Is that the procedure through which I can allocate the heat source?

1) Initialization
2) File/Read/Profile

By the way, Are you sure that a profile could be used for specifying volumetric heat source?
When I want to write a profile, it is just applicable for surfaces and boundaries and that is why that I am dubious about using such option for volumetric heat source.


Thank you in advance
Best Regards

[AlexanderZ]

format is this

((n point 3)
(x
0.023571428
0.030714285
0.037857141
)
(y
0.0099999998
0.0099999998
0.0099999998
)
(z
0.12
0.12
0.12
)
(total-energy
1611.35
1611.35
1611.35
)
)

instead of name"total-energy" you may use ANY name you prefer
idea is for each point you are defining heat source

of course the best is to define heat source for each center of finite volumes

read profile first, apply it in cell zone conditions as a heat source
initialize

[sasanghomi]

Thank you Alexander.

Just one question;
Are the values of heat sources in the table counted per volume? I mean the values of heat sources in the table will be multiplied by cell volumes and will be allocated to the domain?

So, does it mean that the total heat source would change if I changed the grid size?

I would be thankful if you could clarify it.

[AlexanderZ]

values are in W/[m3]
but the volume here means volume of zone, where profile is applied
so you can change mesh

[sasanghomi]

Dear AlexanderZ

Following our recent discussion, I have another question.
I have a profile in which 3,000,000 points have been used to generate the profile. Something weird is happening. The process of initialization is too time-consuming. it is more than 4 hours that I have been waiting for the initialization.
The simulation includes 12,000,000 grid cells and it is a just conduction heat transfer modeling.
Do you have any ideas about this issue?

I appreciate your attention.