[mangili]

Hello everyone,

I am conducting a study on cooling punches using forced ventilation, and I need to determine the average convective heat transfer coefficient on the object. I designed the punch in SolidWorks and exported it to SpaceClaim, where I placed an enclosure around the object. After setting up the enclosure, I removed the solid object. Then, I opened the MESH and applied a body sizing condition to the entire domain, a face sizing condition to the walls of the object, and an inflation condition on the object. Afterward, I named all the faces as Inlet, Outlet, Symmetry, Wall, and Object (which represents my punch). For the Object condition, I set a temperature of 90°C using an equation, and I parametrized the Workbench to run several simulations at different temperatures such as 80, 70, 60, down to 30°C. I also used an equation to monitor the convective coefficient on the object's walls.

In theory, as the temperature decreases, the coefficient should also decrease. However, what is happening is that the wall temperature decreases, but the coefficient stays the same or even increases. I have no idea what else to try to fix this . Does anyone know what could be causing this?

[Opaque]

Originally Posted by mangili

Hello everyone,

I am conducting a study on cooling punches using forced ventilation, and I need to determine the average convective heat transfer coefficient on the object. I designed the punch in SolidWorks and exported it to SpaceClaim, where I placed an enclosure around the object. After setting up the enclosure, I removed the solid object. Then, I opened the MESH and applied a body sizing condition to the entire domain, a face sizing condition to the walls of the object, and an inflation condition on the object. Afterward, I named all the faces as Inlet, Outlet, Symmetry, Wall, and Object (which represents my punch). For the Object condition, I set a temperature of 90°C using an equation, and I parametrized the Workbench to run several simulations at different temperatures such as 80, 70, 60, down to 30°C. I also used an equation to monitor the convective coefficient on the object's walls.

In theory, as the temperature decreases, the coefficient should also decrease. However, what is happening is that the wall temperature decreases, but the coefficient stays the same or even increases. I have no idea what else to try to fix this . Does anyone know what could be causing this?

Would you mind putting the equations you mean by convective heat transfer coefficient? Something seems off with your expectations.

[mangili]

Originally Posted by Opaque

Would you mind putting the equations you mean by convective heat transfer coefficient? Something seems off with your expectations.

Thank you for responding.

This is the solid for which I need to measure the convective coefficient. I'm using the following equation for convective heat transfer:

(areaAve(Wall Heat Flux)@Solid) / (area()@Estampo) * (areaAve(temperatura)@Solid - (areaAve(temperatura)@Inlet))

Additionally, I have also used this equation:
areaAve(Wall Heat Transfer Coefficient)@Estampo

However, the second equation does not change the results when the temperature of the solid decreases, and I'm not sure if my reasoning about the problem is correct.

PS: Actually, my object is not a solid. When I created the geometry in SpaceClaim, I removed the solid, leaving only the surface shape. I am considering the walls of the object as a solid. Is my thinking right?

[Opaque]

Originally Posted by mangili

Thank you for responding.

This is the solid for which I need to measure the convective coefficient. I'm using the following equation for convective heat transfer:

(areaAve(Wall Heat Flux)@Solid) / (area()@Estampo) * (areaAve(temperatura)@Solid - (areaAve(temperatura)@Inlet))

Additionally, I have also used this equation:
areaAve(Wall Heat Transfer Coefficient)@Estampo

However, the second equation does not change the results when the temperature of the solid decreases, and I'm not sure if my reasoning about the problem is correct.

PS: Actually, my object is not a solid. When I created the geometry in SpaceClaim, I removed the solid, leaving only the surface shape. I am considering the walls of the object as a solid. Is my thinking right?

Your expression has too many assumptions that could get you into trouble at some point.

Formally, the formal use of the heat transfer equations should be:

Total Wall Heat FLOW = integral over the surface of local heat flux = integral over the surface of ( H * (T_inlet - T_wall))

If you assume the heat transfer coefficient does not change over the surface, or want to compute an average of it, you can factor it out of the integral and have your expression

H = Total Wall Heat FLOW / (integral over the surface of (T_inlet - T_wall))

Now using Ansys CFX CEL, you define an expression for the "local temperature difference at a face respect to your reference (inlet)":

MyLocalDeltaT = areaAve(Temperature)@Inlet - Temperature

MyHeatCoeff = areaInt(Wall Heat Flux)@Wall / areaInt(MyLocalDeltaT)@Wall

[mangili]

Originally Posted by Opaque

Your expression has too many assumptions that could get you into trouble at some point.

Formally, the formal use of the heat transfer equations should be:

Total Wall Heat FLOW = integral over the surface of local heat flux = integral over the surface of ( H * (T_inlet - T_wall))

If you assume the heat transfer coefficient does not change over the surface, or want to compute an average of it, you can factor it out of the integral and have your expression

H = Total Wall Heat FLOW / (integral over the surface of (T_inlet - T_wall))

Now using Ansys CFX CEL, you define an expression for the "local temperature difference at a face respect to your reference (inlet)":

MyLocalDeltaT = areaAve(Temperature)@Inlet - Temperature

MyHeatCoeff = areaInt(Wall Heat Flux)@Wall / areaInt(MyLocalDeltaT)@Wall

It helped me a lot!
I will do this study now, thank you very much for your help.