CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   a problem of natural convection boundary conditions (http://www.cfd-online.com/Forums/cfx/97522-problem-natural-convection-boundary-conditions.html)

 xlworn February 19, 2012 09:58

a problem of natural convection boundary conditions

:confused:
http://img2081.poco.cn/mypoco/myphot...9212847055.png
I want to solve a problem like this，water in cylindrical tank at 293.15K，and a single tube located in the center of the tank，I choose fixed wall temperature of tube at 363.15K，for reducing the calculation，I just modeled 1/4 of tank. My working fluid is water 97 in library of CFX 12, when i choose that，CFX choose full bouyance model，so without boussinique model. i set gravity accelerate 9.8, ref density 1000kg/m3.

At first，I set heating tube wall as fixed temperature wall，and adiab wall conditions both at bottom and tank wall，also at the top free surface，but i cannot get result，Imbalance of H-energy is 100%，i confused maybe energy cannot fulfill conservation rule？but when i changed top free surface boundary condition to fixed temperature wall of 293.15K，it still cannot convergence，also because of H-energy imbalance. calculations are all in transient，about 500s.
And mesh elements about 30000 or 300000 have same result，mesh quality is good.

Then i choose opening boundary for top free surface，in transient calculation i got the result but temperature gradient is so small bulk region is still 293.15K，and i cannot capture the velocity vector.

sincerely hope someone can give me advice，I am a new bird in CFX calculation，and my English is poor.

Thank you!

 ghorrocks February 19, 2012 17:26

I see many problems with what you have said so far:

* For a steady state run you need to balance the heat inputs to the system. Your hot tube is putting heat into the system, so where is it coming out?
* Why did you choose a 90 degree slice? For low Rayleigh numbers (if you don't know what Rayleigh number is then google it, you will need to know it for a simulation like this) the flow is 2D so can be modelled with a very thin slice. But for moderate to high Rayleigh numbers the flow is 3D and it is unlikely you can apply symmetry planes at all.
* For moderate to high Rayleigh numbers the flow will be transient, so a steady state run will not work.
* Rather than trying all sorts of boundary conditions and seeing what works, how about you place boundary conditions appropriate to what you are modelling? What did the experiment you are trying to reproduce do?
* I assume by water 97 you mean the IAPWS mode. Do not use these unless you need the very high levels of accuracy it will give, because they significantly increase the numerical instability are are much harder to converge. Just use standard constant properties water while you are trying things out. Only go back to IAPWS once the simulation works properly and you need the additional accuracy... and have time to sort out all the convergence issues.

 xlworn February 19, 2012 21:27

Quote:
 Originally Posted by ghorrocks (Post 345208) I see many problems with what you have said so far: * For a steady state run you need to balance the heat inputs to the system. Your hot tube is putting heat into the system, so where is it coming out? * Why did you choose a 90 degree slice? For low Rayleigh numbers (if you don't know what Rayleigh number is then google it, you will need to know it for a simulation like this) the flow is 2D so can be modelled with a very thin slice. But for moderate to high Rayleigh numbers the flow is 3D and it is unlikely you can apply symmetry planes at all. * For moderate to high Rayleigh numbers the flow will be transient, so a steady state run will not work. * Rather than trying all sorts of boundary conditions and seeing what works, how about you place boundary conditions appropriate to what you are modelling? What did the experiment you are trying to reproduce do? * I assume by water 97 you mean the IAPWS mode. Do not use these unless you need the very high levels of accuracy it will give, because they significantly increase the numerical instability are are much harder to converge. Just use standard constant properties water while you are trying things out. Only go back to IAPWS once the simulation works properly and you need the additional accuracy... and have time to sort out all the convergence issues.
Thank you very much. I will try to modeling with full partition. The problem I want to simulate is a tank has a free surface in atmosphere pressure. What I concern about is in high rayleigh numbers，I didn't know that symmetry boundary condition cannot be used in high rayleigh numbers.
And I want to know，tank free surface with atmosphere pressure should be simulated in what boundary condition？

 ghorrocks February 20, 2012 01:54

No, the first thing to do is to work out the Rayleigh number. Only then will you know what type of flow you are going to get, then you make the decision of a 3D or 2D mesh from that. What is the Rayleigh number of your flow? If you don't know, then look it up and work it out.

If your top surface is a free surface you have more options. Does the free surface move such that it affects the flow? Does liquid evaporate at it? What is the heat conditions on the other side of the interface - convection with the gas and/or radiation?

 xlworn February 20, 2012 02:47

Quote:
 Originally Posted by ghorrocks (Post 345232) No, the first thing to do is to work out the Rayleigh number. Only then will you know what type of flow you are going to get, then you make the decision of a 3D or 2D mesh from that. What is the Rayleigh number of your flow? If you don't know, then look it up and work it out. If your top surface is a free surface you have more options. Does the free surface move such that it affects the flow? Does liquid evaporate at it? What is the heat conditions on the other side of the interface - convection with the gas and/or radiation?
Rayleigh numeber is about 10^8, tube in the centre of the tank, other walls are adiabatic wall except the top free surface, and the surface don't move, at first i want to calculate without evaporate, but further i need concern about evaporate.
i know that the rule of laminar turn to the turbulance is about Ra=10^8~10^10, but choose different characteristic length will get very different Ra number，for vertical tube when i choose the length of tube for characteristic, Ra number reach 10^15, in some natural convection correlation it is recommended tube length will be appropriate characteristic length. in CFX which one i should choose tube diameter or tube length.
finally, i want to calculate a very long tube, as long as 7 meters. i want to study the variation of boundary layer thickness，and when the water in the tank has formed thermal stratification what difference in heat transfer.
after the calculation of single tube，i need calculated tube bundles horizontal and vertical.
so any recommendation, thank you!

 ghorrocks February 20, 2012 06:14

In that the flow is almost certainly full 3D and transient. You can model the top free surface with a slip wall with a convection boundary condition if you like, this is pretty crude but a reasonable start.

 xlworn February 29, 2012 02:19

I've tried modeling full part of tank with a slender tube in it. Tank with 0.1*0.1*2, and tube with 6mm diameter, bouyance model concerned, water with constant properties, in transient calculation H-energy imbanlance as high as 100% after 30s. I find that temperature gradient appear near the wall within a very thin layer. But I' ve calculated the same problem just with a small cylingderical tank and a relative short tube in it. In transient calculation it has a good result, water in tank formed thermal stratified. I assumed that maybe mesh quality is not good. But I've tried more 。。。。mesh. It still not worked. I want to know if the natural convection heat transfer calculation between a very slender tube with tank can be modeled in CFX?
THANK YOU VERY MUCH!

 ghorrocks February 29, 2012 06:57

If you are getting that high imbalances are you sure your simulation is converged?

CFX can model what you are talking about, the problem is with your set up. It is just a matter of finding the problem.

 All times are GMT -4. The time now is 07:33.