## Fluids

#### Problem between surface area and sum of the element of the same surface

• Aslae
Subscriber

Hey everyone,

Actually working on a free convection simulation problem, physic is doing fine, but I have a problem of incompatibility between my surface area and the sum of the elements of the same surface.

For example, a square surface of 1m^2 : I mesh that surface, do my calculations and I export my datas.

When I check the "surface cell elements" in the exported datas for my wanted surface, and when I sum it, I don't have the area of my surface, which is 1m^2.

Most of the time I have far more than the real surface area. I believe Fluent export all the elements surfaces who have a common plan with the wanted surface.

It is a problem because when my surface is a interface between a fluid and a solid, some of the points of my surface (solid) are fluid, which is not very convenient for calculating thermal coefficient, temperature, Nusselt, etc.

Do you have a idea to help me?

Perfection would be to manage to export datas from the surface without the fluid little mistakes.

It would be to have the same surface area in my datas and for my real surface too.

I am blocked here for almost two weeks, I wasn't able to solve this problem yet.

Thank you very much for your time,

Thomas

• DrAmine
Ansys Employee
What does the Surface Integral "Area" return?
• Aslae
Subscriber
Hello,
I didn't find the surface integral "Area" in the export data window.
I can export the "cell surface area", but I have the problem exposed above, the incompatibility between the area of the real surface (1m^2) and the sum of the meshing elements of the surface (6,18m^2).
How can I be sure that I export all the points of my surface and not from anywhere else?
Because it's my problem actually, I don't really care about the area of my surface, I just want to be sure that all my elements are on my surface and only on my surface.

I'd be quicker now, I had an issue with my internet.

Thank you
• Rob
Ansys Employee
I think you're exporting the data for all facets on the cells on the surface. In the Surface data what area do you get?
• Aslae
Subscriber
I think you're right, the surface data in DesignModeler are right.
I want to export all the datas from a surface (Temperature, h, fluxes, ...), but I'm sure that when I export the datas from a specified surface, I have some datas who aren't from that surface.
Especially, one of my surface is a solid, with fixed temperature, next to a fluid, with a variable temperature, I have datas from both the surface and the fluid next to it.
How can I fix that? I want each and every point of my surface, but nothing else.

Thank you
• DrAmine
Ansys Employee
How are you exporting? Can you try to export in ASCII Format one variable on one particular BC and check the values there?
• Aslae
Subscriber
I'm exporting datas with ASCII Format to an excel, it's where I found that I had a problem with my system.
For exemple, when I set a constant temperature to a surface (300K), do the simulation, then export the datas on that surface, I have some values which are not at 300K, but 301K, 307K, and more.
After another night on the problem, I think the exportation is good, it's my boundary configuration which is not.
I set for the BC of that surface, in Thermal, "Temperature 300K - Constant", How can I do more?
Same thing for my adiabatic walls, I don't think they actually are adiabatic. My isotherms aren't absolutely perpendicular to the surface, but I set them in thermal to "heat flux = 0", I don't know what to do to improve that.
If you want I can send you datas and screenshots of my parameters.
Thank you
• DrAmine
Ansys Employee
You can insert any screenshots here. If you set the wall to constant 300 K which values are exported in ASCII? Is that wall a wall/wall-shadow wall or a wall with only one neighbor?
• Rob
Ansys Employee
Can you also post an image of what you're exporting? If the wall bc is set at 300K the export should be 300K unless you're picking up the near wall cell centre value.
• Aslae
Subscriber
My system is a solid quarter sphere (source 5W) and a Fluid surrounding it.
Here you have my cupola set to 300K constant, my walls horizontal and vertical adiabatic.
• Aslae
Subscriber
Here it is just my cupola, who is not at 300K everywhere, for example in the top you can see a band of higher temperature. It has to be 300K everywhere for my experiment

• Aslae
Subscriber
Same for my source which is a constant volumic source of 5W, this surface has to be uniformly heated too

• Aslae
Subscriber
here my exportation,
For the cupola is a simple wall with a unique neighbour. (above)
Not the same thing for the source surface which is a interface between solid and fluid, so there is a wall/wall shadow for the source.

• Rob
Ansys Employee
Redisplay the contours with node values and global range off
• Aslae
Subscriber
For the cupola
For the source
• Rob
Ansys Employee
Maybe so we can see them? Under File there's a Save Picture option.
Which machine(s) are you using to run the models?
• Aslae
Subscriber
I'm working on a desktop computer and a laptop, but mainly the desktop computers.
source on the top and cupola for the bottom

• Rob
Ansys Employee
OK. I assume gravity is set in the y direction as -9.81m/s/s?
External face is 300K (fixed), source in the solid is 5W and other boundaries are adiabatic. What do you see if you plot the wall temperature on the outer face?
• Aslae
Subscriber
You're right for the settings.
I have for the vertical wall this
and this for the horizontal one
The third one is the cupola that you have already

• Rob
Ansys Employee
OK, this makes more sense now.
Have a look at the flow vectors in the domain. Warm air rises (I assume it's ideal gas) from the heated surface, and takes heat to the top of the domain where it cools and heads back down. When you display the temperature on the walls with node values off you're seeing the facet temperature but it'll also be influenced by the near wall cell temperature. As your mesh is relatively coarse that may excessively alter the surface temperature. Use adaption to adapt the fluid region a couple of times and run the solution on. Then compare the results.
• Aslae
Subscriber
Okay, yes, it's really helpful, I think it will be alright after few adjustments.
Thank you so much