Learning Forum

[Shruti_15]

I am performing a 2D natural convection analysis on a horizontal plate in fluent flow (fluent). The boundary condition are:

constant heat flux, applied on the upper edge of the plate,

constant temperature equal to 300 K on all edges of the control volume.

The flow is visible but the plate is not heating.

[Sanskriti_33]

Same problem please tell the solution

[srishchai]

Hi, IÔÇÖm facing the same problem for quite a time now.
Instant help will be appreciated.

[Rob]

The contour looks "odd". How many volumes do you have, and what did you assign as the surface type (and settings) on the wall that's common to both zones?

[Shruti_15]

I have 2 volumes, fluid domain (control volume) and plate domain (plate).
On Wall fluid domain and wall-plate domain I applied the same value of heat f lux.
I have attached the display window of these two domains.

[Rob]

You need a coupled wall between the two zones or an interface (the former is better). Not sure what's going on in the solid, can you replot with node values off?

[Shruti_15]

I am not getting the option of coupled in boundary conditions, and when I'm making it an interface then it's not initializing.

[Rob]

OK, go back to geometry and check you have a multibody part or did share topology. Check in Meshing for "contact" regions and make sure they're correct. If there's a fault when you initialise, what is it? You then apply the heat to the solid, or in the coupled wall (you'll need to give it a thickness). Or omit the solid and just add the flux to the surface where the solid would have been.

[Shruti_15]

I have added shared topology and the contact regions are correct too. But in fluent these walls are created and in display option, no region is being displayed for these walls.

[Rob]

Can you post an image showing each of the interface regions separately? There's something odd here as share topology should mean you don't have any contact regions.

[Shruti_15]

Okay earlier there were contact regions . But now I have again added shared topology, when I display body by connections this is what it displays Then in mesh there were no contact regions and i have attached a pic of my mesh and named selections, the heatfluxwall is the upper edge of the plate where i want to apply heat flux condition..
Then in mesh I applied constant heat flux of 1000 W/m^2 to heatfluxwall and it's shadow. And part_surface_body was created by fluent which is the remaining sides of the wall (left, right and bottom) to which i applied coupled boundary condition. Now when I run my simulation the flow is coming from only the top surface of plate (where I have applied heat flux).
I want to see temperature in the plate and also the flow should be coming from the lower part too.

[Rob]

Zoom right in and check. You may want to display temperature on the fluid only.

[Shruti_15]

I applied the coupled wall and everything you said and the plate turned red. But there's another problem I am formulating the problem of applying 1000 W/m^2 of heat flux on the upper face of plate in 3D. What should be heat flux that I should apply on the upper edge of the 2D here.
Right now i am applying a flux of 1000 to simulate, but the heat transfer coefficient that fluent is reporting is 5.1 W/m^2 K. When I am calculating this theoretically by empirical formulas, it is coming 8.5. Where do you think the problem could be?

[Rob]

Why are you setting the heat flux on the wall? The whole point of the COUPLED wall is that heat is passed from the solid to the connected cell zones.
HTC is a made up number used to compare data between designs. Check that the reference you're using in Fluent is the same as the empirical formulation. Also check what the formula has to say about the end effects of the plate.