[Antanas]

Originally Posted by Ethan_Sparkle

Hi Erik, it seems you proposed a promising way to do this, I get what you mean, but I do not quite understand how to achieve that. Could you please explain it in detail? or any reference thread. I find it difficult to look for the related post without understand it.
How can I specify the fluid is cooled by the same amount?
yeah, the inlet temperature profile (not the uniform 300K) should be something associated with the velocity profile, with its bulk temperature is 300K. How can I get that inlet temperature profile?
In the fluent results, everypoint temperature value in the outlet is the corresponding point temperature value in the inlet plus the same delta T.
Horrocks, I don't manage to achieve this using the additional variables. You can see the eqution 14-22 in former post picture, I guess I need to find the T profile of the inlet, while knowing the velocity profile and bulk temperature. Kind of impossible to do this with out using fortran to do some iteration work.
Any convenient idea?

I think he meant that you should
1. Create CEL expression Tbulk = areaInt(T * density * Velocity)@inlet / areaInt(density * Velocity)@inlet.
2. Create Monitor of Tbulk.
3. Set constant energy source term at inlet, say 100W.
4. Start calculation.
5. During calculation use "Edit Run in Progress" functionaity to change source term value so that your monitor for Tbulk come to 300 K.

[Ethan_Sparkle]

Originally Posted by Antanas

I think he meant that you should
1. Create CEL expression Tbulk = areaInt(T * density * Velocity)@inlet / areaInt(density * Velocity)@inlet.
2. Create Monitor of Tbulk.
3. Set constant energy source term at inlet, say 100W.
4. Start calculation.
5. During calculation use "Edit Run in Progress" functionaity to change source term value so that your monitor for Tbulk come to 300 K.

Hi Antanas, thanks for your explanation. I think that's exactly what Erik meant. I tested this method in a periodic tube. However, it seems it only work for specified temperature boundary, not for a heat flux one.
For the specified temperature case,
there are still some problem in the inlet and outlet part. the first picture is the fluent result.

while this one is the CFX result


For the heat flux boundary case, when you set the source term to be the "Wall heat flux*Wall area/inletarea", you can get a convergence value for the inlet bulk temperature , which is around 280K; when you set other value for the source term, then the bulk temperature are always increasing or decreasing.

[evcelica]

Yes, The method I described would not be balanced if using heat flux as a wall condition since there is no temperature anywhere to bound the problem. For that you would want to put in an expression along the lines of:

MyConstant * (MyDesiredTemp - TempBulk)
where "MyConstant" is something like 100[W/K] or more maybe.
and "TempBulk" is massFlowAve(Temperature)@Domain Interface 1 Side 1. (or whatever you deem appropriate)

This method would work with both constant Temperature walls as well as heat flux walls. I didn't want to make it too difficult to start with, which is why I just suggested to start using a single value.

I think you may be getting that weirdness at the inlet/outlet because you are displaying Hybrid Temperatures, and it's making some improper assumption about the interfaces hybrid temperature because of the source terms. Plot the conservative values instead, and it should look much better.

[Ethan_Sparkle]

Thanks for your help, Erik. However I do not quite understand what "MyConstant *(MyDesiredTemp - TempBulk)" means here. Do you mean use this expression as a source term in the inlet boundary? see if I hope the inlet bulk temperature is 300K. I guess 300K is MyDesiredTemp. So the expression is "MyConstant*(300[K]-TempBulk)". Then monitor the "TempBulk" during iteration and Edit "MyConstant" in Progress? Did I get this right? But if the TempBulk is approaching 300K, then the expression is approaching 0.
What's the hybrid temperature and conservative temperature? I can only find temperature and total temperature in the CFD-Post, and they give the same result. How can I plot the conservative value other than hybrid temperature?
So many questions. Really appreciate for the help.

[evcelica]

Originally Posted by Ethan_Sparkle

However I do not quite understand what "MyConstant *(MyDesiredTemp - TempBulk)" means here. Do you mean use this expression as a source term in the inlet boundary?

Yes put that in as your source term, you are understanding everything correctly. The exact same way you put in the Dirichlet Boundary Conditions Glenn suggested to make the inlet a uniform 300K.

Originally Posted by Ethan_Sparkle

What's the hybrid temperature and conservative temperature? I can only find temperature and total temperature in the CFD-Post, and they give the same result. How can I plot the conservative value other than hybrid temperature?

In CFD-post, just look for the hybrid vs. conservative vales in the advanced options when defining a contour plot.

[Ethan_Sparkle]

Yes, you are totally right about that, I changed to conservative values and the results contour are quite similar with the fluent results.
Using that expression as the source term, when the bulk temperature is approaching my desired temperatuer, say 300K, then the expression will approach zero,which means the source term is zero then. Don't understand that.

[Ethan_Sparkle]

Anyway I tried this for the heat flux wall boundary case, but did not get a result. I used the expression "(-1000*(300[K]-Tbulk)/1[K])[W m^-2]" as the inlet source term. But ths monitored Tbulk curve went all the way to 10^20.

As I said, still don't understand what this expression mean as a source term. Could you please explain a litter further about this?

[evcelica]

Looks like you added an extra negative sign in there for some reason, that would cause a runaway boundary condition, pushing it further and further from your desired temperature.... pretty much doing the exact opposite of what you want to do. Your constant should be positive.

Yes, the expression will approach zero as you approach your desired temperature so you will always have an offset, which is inversely proportional to your constant. You can add additional cooling in there to reduce this offset, or just change your desired temp. There are many ways to fix that small offset. Post processing the results included.

[Ethan_Sparkle]

Thanks Erik, I have tried so many different combinations about the simple periodic tube heat transfer problem. The tube is subjected to a constant heat flux in the wall.
I noticed you edited your last post which mentioned "I believe that with constant fluid properties, a single simulation can be valid for all inlet/bulk temperatures. The energy term is a linear scalar. You just have to understand and post-process the results properly using valid pi groups." Could you please explain this a little more? what is "pi groups"? And also what do you mean by "post processing the results included"
In fluent, I get the result like this. Also the temperature profile at the inlet and outlet have the same shape only with a value offset, which is very reasonable, as the relation between the temperature profile at the inlet and outlet is Toutlet=Tinlet + dT*L.

Also, if a source term related with the constant heat flux is added, the periodic part the the temperature should be obtained like this,

However, in CFX, when I define a source term "-1000000*(Tbulk/1[K]-300)[kg m^2 s^-3]" in the inlet position to pull the inlet bulk temperature to 300K. Tbulk=massFlowAve(T)@inlet. I got the following result, the shape of the inlet and outlet temperature distribution are not the same.

I also tried the same source term in the outlet position, but got a even stranger result,

I could not figure out which part is wrong. Anyone can help me with this? Thank you very much for all your help.

[Ethan_Sparkle]

As far as I understand, I guess the source term "-1000000*(Tbulk/1[K]-300)[kg m^2 s^-3]" used in inlet is used to pull the inlet bulk temperature to 300[K], which should lead to the similar results with that of the fluent case.
And plus one more source term related with the constant heat flux, a periodic temperature contour should be obtained, which have same value for inlet and outlet position, in this specific case, i.e. same temperature profile in every section.

[evcelica]

I thought I explained this already, don't make the inlet 300K, cool the inlet by a uniform amount, which will give you a periodic temperature condition, just like the Fluid results. It is analogous to pressure in periodic flow.

I meant you can perform one simulation and predict the exact solution to other inlet temperatures and wall heat flux values using data you obtained from the first solution. Temperature is a linear scalar (with constant fluid properties) and can be scaled accordingly if you do the post processing right. Pi groups are used in dimensional analysis, or similitude.

[Ethan_Sparkle]

Hi Erik, I did use the Tbulk=massFlowAve(T)@inlet in the source term expression "-1000000*(Tbulk/1[K]-300)[kg m^2 s^-3]", which I think will set the inlet bulk temperature(related to the flow field) to 300K, not a uniform one. I guess this is what you mentioned before. I did think this would work, however, I got the results in my last post. Don't understand which part is wrong.

[evcelica]

What are the dimensions of your model?
Flow rate?
Fluid Property?
Wall Temperature or Heat flux?

It looks like your two simulations for inlet vs outlet boundary source would look the same if you plotted conservative values instead of hybrid.

[Ethan_Sparkle]

I do plot the conservative value for both cases. I just modeled a simple tube with radius=0.05m, length=0.2m, set the inlet and outlet to be periodic interface and define the mass flow rate=0.001kg/s, a constant heat flux=1000W/m^2 was put in the tube wall. Water is used in my model. I chose the laminar. Since there is no place to define the inlet temperature in the periodic interface, so a source term "-1000000*(Tbulk/1[K]-300)[kg m^2 s^-3]" was used.
I put the source term in either inlet boundary or outlet boundary, but got the two different result like the post before. The inlet case makes much more sense, but the temperature distribution shape are not the same for the inlet and outlet position, while is different with the fluent result.

[Ethan_Sparkle]

Anyone has any idea or hint which part I might be wrong? I thought it should give the right result when a source term like that was added, however, it didn't. Many thanks.

[evcelica]

I was thinking about this, and we want to cool all the fluid by the same amount, meaning drop the temperature by the same amount everywhere as it passes through the interface. I was thinking uniform source would do this, but that would cool the slower moving fluid too much, and faster moving fluid not enough, if it does this as a flux.

I believe we need to include velocity into the equation:
something like:
MyConstant * (MyDesiredTemp - TempBulk) * (Velocity / massFlowAve(Velocity)@Domain Interface 1 Side 1)
where "MyConstant" is something like 1[W/K] or more maybe.
and "TempBulk" is massFlowAve(Temperature)@Domain Interface 1 Side 1. (or whatever you deem appropriate)

[Ethan_Sparkle]

Many thanks Erik, I tried this idea, but it did not make any differences. Actually I think the velocity is already considered when defining the Tbulk=massFlowAve(Temperature)@inlet. Couldn't see any reason why the temperature distribution in the section is not right, they should have had similar shape when under constant heat flux. So confused

[Ethan_Sparkle]

Also Horrocks, I remeber you said in order to prevent the fluid from being warmed up all the time, a source term should be added to take away the same amount of heat translated from the wall. However, when I used the source term "-1000000*(Tbulk-300[K])", It just set the inlet temperature, while it did not take away the same amount of heat that was from the wall. What happened here? Could you please say more about this? Thank you very much.

[Ethan_Sparkle]

I'll just saying something that may clarify the problem more clearly.
In Fluent, the both periodic flow and heat transfer can be modelled. For the constant heat flux case, the inlet temperature profile and the outlet temperature profile should have the same shape with a offset, which can be seen below.

The red one for the inlet T profile, while the blue one for the outlet T profile. Here the inlet bulk temperature is set to be 300K.
However, in CFX, even though I defined Tbulk=massFlowAve(T)@inlet, and used the source term "-1000000*(Tbulk/1[K]-300)[kg m^2 s^-3]" in order to set the inlet bulk temperature to be 300[K], the reslut is still like a uniform inlet temperature 300[K], which can be seen below.

The red on for the inlet T profile, and the blue one for the outlet T profile. It can be seen that the inlet T is almost a uniform 300K.
The bulk temperature is defined by ,
actually if it has a uniform T=300K, we can still get the Tbulk=300K. So the CFX results is to some extent right. In order to confirm my thought, I first calculate the flow only, can export the outlet velocity profile, then set the boundary as "inlet and outlet" instead of "periodic interface", and import the velocity profile as the inlet boundary, with a fixed 300K temperature, than calculate the heat transfer only. I got the following result.

It is almost same with the periodic one with a source term.
So the question is how can I restrain the inlet bulk temperature to have the same shape with the outlet temperature profile? I was thinking about exporting the outlet temperature profile, minus a dT, and put it to the inlet temperautre profile, and calculate again, maybe after several iterations, I can get a similar result with the fluent one. However, it seems I couldn't import the temperature profile data just the way I did with the velocity profile. There is no such options for temperature input. Only a fixed number or CEL. So is there any way to export the temperature profile as a CEL form?
Please let me know if there is some advice or if I am wrong somewhere. Thank you all.

[Ethan_Sparkle]

Hi everyone, anybody has any idea about how to deal with this problem? Any idea is appreciated