[Hamda]

Hi,
first of all It should be mentioned that I read the following link :
https://www.cfd-online.com/Wiki/Ansy...ficient_in_CFX


But it didn't help me on my problem. My problem is that I want to write an expression for htc as follows:
htc= Wall Heat Flux/(Ts-Tf)
where Ts is solid temperature and Tf is fluid temperature and I already drew charts for solid and fluid temperatures along the axial direction. But when I use the above expression for htc, I get error. Is there anybody who knows how can I solve my problem? since Ts and Tf change along the axial direction and I couldn't use constant temperature.
Many thanks in advance.

[Gert-Jan]

In my opinion, you are trying to do thing that are not possible.
Nu and h relations are based on simple ideal systems (flat plate, straight pipes) with constant temperatures on large distances, and not a complex geometry like you have. Since Tf and Ts change, there are no reasonable value.
The only thing you can do is use masflow averaged values from your main inlet to main outlet or over sections of your geometry, bounded by an inlet plane and outlet plane.

[urosgrivc]

If you want to get HTC based on a fixed external temperature you should change the T-bulk parameter in expert parameters to a fixed temperature in [K]

[Hamda]

Originally Posted by urosgrivc

If you want to get HTC based on a fixed external temperature you should change the T-bulk parameter in expert parameters to a fixed temperature in [K]

I already know it but what about T-hot?? it should be constant too? along the axial direction T-hot changes and its change effects htc.

[Gert-Jan]

As mentioned, in my opinion, you are trying to do thing that are not possible.


You can take the temperature in the center of each sphere and subtract the average fluid temperature on the same stage. In other words, define your own Nu number.....

[evcelica]

Read the FAQs again. You need to make an expression for fluid temperature "MyBulkTemperature" It will be a function of what appears to be Y in your case, if that is how you would like to define the fluid bulk temperature. Then make an expression for MyHTC = Wall Heat Flux/(T-MyBulkTemp). Makje a variable from this expression.

Plot this on the solid side of the interface.

Or use the approach in the faqs to get "wall temperature" and you could plot it on the fluid side of the interface. If you try to use T on the fluid side, in an expression, it will use the conservative value (adjacent node) not the hybrid wall temperature.



But as Gert-Jan hints at, your results may end up looking wierd, as you are really just defining your own Nusselt number.

[Hamda]

Originally Posted by evcelica

Read the FAQs again. You need to make an expression for fluid temperature "MyBulkTemperature" It will be a function of what appears to be Y in your case, if that is how you would like to define the fluid bulk temperature. Then make an expression for MyHTC = Wall Heat Flux/(T-MyBulkTemp). Makje a variable from this expression.

Plot this on the solid side of the interface.

Or use the approach in the faqs to get "wall temperature" and you could plot it on the fluid side of the interface. If you try to use T on the fluid side, in an expression, it will use the conservative value (adjacent node) not the hybrid wall temperature.



But as Gert-Jan hints at, your results may end up looking wierd, as you are really just defining your own Nusselt number.

Dear evcelica,
Thank you for your response. I already defined an expression for MyBulkTemp I just wondering can I use this epression in CFD post or I have to back Pre CFX ?

what do you mean about htc expression? Can I use "MyHTC = Wall Heat Flux/(T-MyBulkTemp)" as the expression?
Also I want to show Nusselt number distribution on a selected sphere. How can I do that? I should insert a volume(sphere volume)? and draw a contour of it?

[evcelica]

You can do this all in POST.

HTC is a surface variable, so you only want to display it on the surfaces (fluid solid interfaces). Which side of the interface you display it on will give different results, so make sure your variable definition if consistent with your chosen display location.



You must make the expression, then a variable based on that expression in order to make a contour plot of it. You can't make contour plots of expressions, only variables.
Make an expression in CFD post using the directions I gave you, and in the FAQs.
If you only want to show it on a particular sphere only, and not the whole interface, you can try choosing mesh locations as the location of the contour plot, and just choose that mesh location.

[Hamda]

Originally Posted by evcelica

You can do this all in POST.

HTC is a surface variable, so you only want to display it on the surfaces (fluid solid interfaces). Which side of the interface you display it on will give different results, so make sure your variable definition if consistent with your chosen display location.



You must make the expression, then a variable based on that expression in order to make a contour plot of it. You can't make contour plots of expressions, only variables.
Make an expression in CFD post using the directions I gave you, and in the FAQs.
If you only want to show it on a particular sphere only, and not the whole interface, you can try choosing mesh locations as the location of the contour plot, and just choose that mesh location.

Thank you. Now I can get contours, but I get negative values for nusselt number!! I don't know how can I fix it.

[evcelica]

That is because this is a complex geometry, and your fluid bulk temperature is a complex 3D field. Really it does not have a real standard definition for a complex geometry like this. For a pipe, it would be massFlowAve(T)at that cross section. But for this geometry, that probably isn't applicable. How did you define it?
The that is why the standard HTC variable in CFX just used wall adjacent node temperatures for the fluid temperature. but that value it gives will be completely mesh dependent.

What you could do is find the average HTC for the entire interface using average values of heat flux, wall temperature, and average of Inlet/outlet temperatures.

If you wanted a plot, you could scale the default HTC so that its average matches your Average HTC you calculated from average properties.

But there is no real way to get a true answer in a 3D plot, as Gert-Jan stated before:

Originally Posted by Gert-Jan

In my opinion, you are trying to do thing that are not possible.
Nu and h relations are based on simple ideal systems (flat plate, straight pipes) with constant temperatures on large distances, and not a complex geometry like you have. Since Tf and Ts change, there are no reasonable value.
The only thing you can do is use masflow averaged values from your main inlet to main outlet or over sections of your geometry, bounded by an inlet plane and outlet plane.

[hitzhwan]

Originally Posted by urosgrivc

If you want to get HTC based on a fixed external temperature you should change the T-bulk parameter in expert parameters to a fixed temperature in [K]

I have put the [K], but it give the error again.Why?

[urosgrivc]

did you read, more...?
what does it say?

I think that your expression doesn't work because it is not dependant on location, which htc is, so at least one element in the expression needs to e location dependant.
Did you see this?... I think that you are trying to get point nr.2 from bellow to work a?


Calculating the Heat Transfer Coefficient in CFX
The Heat Transfer coefficient calculated by CFX will be quite different from standard film coefficients calculated by other means, but it is possible to output values that reflect the standard definition.

In CFX, the Wall Heat Transfer Coefficient = Wall Heat Flux / (Wall Temperature - Wall Adjacent Temperature) Most standard engineering equations we are familiar with use some "bulk temperature" in place of the Wall Adjacent Temperature. Of course, CFX has no idea what your "bulk temperature" would be, and must use some other value. When using Wall Adjacent Temperature, which is the fluid temperature of the first fluid node off the wall, the returned value for HTC is going to be completely mesh dependent. Where coarser meshes will give you answers approaching the standard definition using bulk temperature, and a fine mesh would give you very large values, as the denominator of the HTC equation is approaching zero.

If you want the HTC to use a different value for the Reference Temperature instead of Wall Adjacent Temperature, there are a two approaches:

1 Use the expert parameter "Tbulk for HTC" and set this to your some reference temperature. CFX will now calculate: Wall Heat Transfer Coefficient = Wall Heat Flux / (Wall Temperature - Tbulk for HTC)

2 Create your own expression for MyBulkTemperature through the geometry, for example, along the pipe length, which may be a function of the length.
Create a new expression for MyHTC = Wall Heat Flux / (Wall Temperature - MyBulkTemperature).
The tricky part is how do you get "Wall Temperature"? Well from the original HTC equation, we can see: Wall Heat Transfer Coefficient = Wall Heat Flux / (Wall Temperature - Wall Adjacent Temperature) Rearrange this equation to: Wall Temperature = (Wall Heat Flux / Wall Heat Transfer Coefficient) + Wall Adjacent Temperature
You can then make a new variable from your "MyHTC" expression, and make a contour, or plot it on a graph with a line running along the wall. Remember this is a boundary only variable.
The same approach can be used for Nusselt numbers as well.