[sasanghomi]

Dear Friends,

I am trying to import heat source at cell centers. The problem is that I do not want to use profiles because it interpolates among different given figures. In fact, I have cell center positions and their corresponding heat sources (W m^-3). So, there is no need for interpolation. However, I have no idea that how I can specify it in CFX.

Do you have any recommendations?

I appreciate your attention.

[sasanghomi]

Following to my first question,
Is there any methods through which I can specify a list of coordinates and heat sources in order to import them as heat source point?
In fact, I want to import heat sources for each cell.

Any ideas is appreciated deeply.

[Opaque]

It seems you are trying to do something in CFX you already did elsewhere, correct? CFX does not uses the "cell" vocabulary anywhere because being hybrid control volume based finite element method it leads to confusion.

When you say center of the cell, are you referring to the center of the element in the provided mesh, or the center of the control volume around a vertex of the provided mesh. They are very different locations and concept from the numerics point of view.

Now to the mechanics of what you are trying to achieve. If you want to impose a heat source directly to the control volume, you create a text file following documentation guidelines where you list

x, y, z, heat source value

the values for x,y,z must be location of the vertices of the provided mesh.

Import the text (.csv) file into CFX-Pre,
Create a subdomain for the mesh volume you are interested in
Activate Energy source term
Set the Source = MyProfile.heat source value(x,y,z)
Apply,

Since you are providing the source at the mesh location, there is no interpolation influence in your results, i.e. it is a null operation since the value will be found in the file.

[sasanghomi]

Thanks for your reply and comprehensive explanation.
However, when the data has dramatic changes, there will be a tangible error even if data is given in nodes.
For instance:

[Name]			
Domain 1			
			
[Spatial Fields]			
X	Y	Z	
			
[Data]			
X [m]	Y [m]	Z [m]	Loss [W]
0.13333	0.066667	0.066667	1
0.13333	0.066667	0.13333	100
0.066667	0.066667	0.066667	30
0.066667	0.066667	0.13333	250
0.13333	0.13333	0.066667	2

You can never dissipate 383 Watt from the surface of a volume whose nodes are provided with the above-mentioned heat sources, if you use a profile. (even if the coordinates are the positions of the nodes)

[Opaque]

Either I got your question wrong, or I did not explain myself clearly.

If you have just a few points, i.e. tens of, just add them one at a time, and there is no interpolation or other sources of errors. If you plan to add total heat flow, use the Total Source option instead. For those script inclined, you can create a script that read a profile file, and create CCL for a

Loop over the number of rows in the [Data] section of the profile
DOMAIN: My Domain
SOURCE POINT: Point $n
Option = Cartesian Coordinates
Write the location from the row in the profile here
EQUATION SOURCE: Energy
Option = Total Source
Write the Total Source Strength in the profile here
END
END
END

You can the merge the CCL at the start of the simulation.

If you have too many to do it manually, and you really want to use a profile file, then you MUST include every single node in the mesh such as there is no interpolation and assign 0 [W] where there are no sources, and non-zero values where you want them to be.

If you use the Total Source option and avoid the interpolation, you can be certain the total energy will be inserted into the volume, not a 1 [W] more, nor one less.

ANSYS CFX does not have a "Cloud of Source Points" option such as only those points in the profile file are used for the source locations.

Hope the above helps you further in realizing your simulation

[sasanghomi]

Thank you Opaque.
Are you sure about it? I am capturing something else compared to your explanations.
I generated a box like the picture attached. All nodes are mentioned in the profile text.
The sum of heat sources is supposed to be 3588 [w]. I specified a convection boundary condition for the box and I ran the case. But the value of "areInt(Wall Heat Flux)" on the boundary is totally different compared to 3588 [w].
What is the reason for that?

[Name]			
Domain 1			
			
[Spatial Fields]			
X	Y	Z	
			
[Data]			
X [m]	Y [m]	Z [m]	Loss [W]
0.13333	6.67E-02	6.67E-02	1
0.13333	6.67E-02	0.13333	100
6.67E-02	6.67E-02	6.67E-02	30
6.67E-02	6.67E-02	0.13333	250
0.13333	0.13333	6.67E-02	2
0.13333	0.13333	0.13333	10
6.67E-02	0.13333	6.67E-02	2
6.67E-02	0.13333	0.13333	200
6.67E-02	0.13333	0	340
0.13333	0.13333	0	22
6.67E-02	6.67E-02	0	11
0.13333	6.67E-02	0	111
0.13333	6.67E-02	0.2	0
6.67E-02	6.67E-02	0.2	0
0.13333	0.13333	0.2	0
6.67E-02	0.13333	0.2	0
6.67E-02	0	0.2	0
0.13333	0	0.2	0
0.2	0	0.2	0
0.2	6.67E-02	0.2	0
0.2	0.13333	0.2	0
0.2	0.2	0.2	0
0.13333	0.2	0.2	0
6.67E-02	0.2	0.2	0
0	0.2	0.2	0
0	0.13333	0.2	0
0	6.67E-02	0.2	0
0	0	0.2	0
0	6.67E-02	0.13333	23
0	6.67E-02	6.67E-02	43
0	0.13333	0.13333	9
0	0.13333	6.67E-02	88
0	6.67E-02	0	67
0	0.13333	0	34
0	0	0	21
0	0	6.67E-02	66
0	0	0.13333	98
0	0.2	0	5
0	0.2	6.67E-02	43
0	0.2	0.13333	23
0.13333	0.2	0.13333	12
6.67E-02	0.2	0.13333	34
0.13333	0.2	6.67E-02	90
6.67E-02	0.2	6.67E-02	100
6.67E-02	0.2	0	123
0.13333	0.2	0	432
0.2	0.2	0	11
0.2	0.2	6.67E-02	0
0.2	0.2	0.13333	0
0.2	6.67E-02	0.13333	0
0.2	0.13333	0.13333	0
0.2	6.67E-02	6.67E-02	34
0.2	0.13333	6.67E-02	21
0.2	0.13333	0	987
0.2	6.67E-02	0	4
0.2	0	0	33
0.2	0	6.67E-02	0
0.2	0	0.13333	0
0.13333	0	6.67E-02	0
6.67E-02	0	6.67E-02	45
0.13333	0	0.13333	2
6.67E-02	0	0.13333	56
0.13333	0	0	3
6.67E-02	0	0	2

[Opaque]

1 - I assume all the other walls are adiabatic, correct?
2 - I would use areaInt(Heat Flux)@Boundary instead
3 - I would look in the output file for the diagnostics/Flow Summary for the energy equation, it should list the amount of heat introduced,


Name of Subdomain -----> Amount
Name of Boundary ------> Amount

You can verify each flow introduced or removed at boundaries and volume. Do you see the source reported exactly (it better be)?