
[Sponsors] 
October 12, 2011, 08:01 
Issues with an attempt to model an inline tube bank

#1 
New Member
Andrew Muharib
Join Date: Aug 2011
Posts: 3
Rep Power: 7 
Hi all I am very new to using STAR CCM+ and was wondering if some one could help me with my dilemma. I have both a Hi and Low Re meshes designed to model flow through a 2x2 inline tube bank. I am modelling the turbulent flow through the 3D system by including periodic boundaries on x, y and z directions. Essentially trying to observe the pressure, coefficient of pressure, and nusselt number around the central tube. The model description is presented below:
Model Considered  Constant Density Gas  Air High y+ wall treatment Implicit Unsteady RANS Reynolds Stress Model Quadratic Pressure Strain (which is the same as SSG) Segregated Flow and Fluid Temperature Three Dimensional Turbulent Air properties: Density = 1.0 Dynamic viscosity = 2.43902439 x105 (1/Reynolds number) and Re = 41,000 Specific heat = 1009 Thermal conductivity = 0.0024609756 (viscosity x specific heat) Turbulent Prandtl Number = 1.0 Initial conditions: Pressure = 0.0 Static temperature = 500K Turbulence intensity = 0.03 Turbulent velocity scale = 1.0 Turbulent Viscosity ratio = 10 Velocity = 1.0 Reference Values: Min allowable wall distance = 1.0 x 106 Min allowable temp = 500 k ( I know this is completely unrealistic however I am using temperature as a passive scalar so it really has no knock on effect to the density and rest of the calculation) Max allowable temp = 5000k Reference Pressure = 0.0 I am struggling with a few problems: 1) Defining the correct stopping criteria and time step for the implicit unsteady solver. 2) I have managed to simulate pressure differences with the simulations I have run so far, however I cannot seem to get the nusselt number plots to work correctly i.e. I get nothing. 3) I am essentially trying to model an inline tube bank, hence the periodic boundaries. I have set the y and z  periodic boundaries with a zero pressure jump. Yet the x  direction periodic boundary has been defined with a mass flow rate of 0.12 kg/s in order to drive the flow. I was wondering if this approach was correct. Any help would be greatly appreciated. Thank you. 

October 12, 2011, 09:02 

#2 
New Member
Andrew Muharib
Join Date: Aug 2011
Posts: 3
Rep Power: 7 
I've added a picture of the model considered.
Thank you. 

October 15, 2011, 11:27 

#3 
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
3. It works, but it doesn't have to be more realistic than a symmetry plane at the Y and Z boundaries.
2. What do you mean with "get nothing"? 1. Choosing the time step and inner iterations is the same like in every unsteady simulation and it already has been discussed at least 50 million times. Choose your time step to keep you convective courant number below one for best results. Check your residuals, best would be if they drop for two or three orders of magnitude in a time step. When they drop too less (let's say less than one order of magnitude in a time step), reduce your time step or increase inner iterations. It might be better to reduce the time step than increasing inner iterations since the accuracy of your results will also improve. And it should be selfexplaning to consider the sampling theorem. Choosing the maximum time stopping criteria is up to you and depends on the physics of the problem and time you want to model (and of course on the computational ressources). I'm wondering why people twiddle with values which are just fine by default, although they 1. Don't need to change this value 2. Know that the value they put is completely unrealistic 3. Seems not to know what this value is good for 4. Don't know about the problems when changing the value 5. Should first concentrate on more important things like time step or boundary conditions Have I missed the start of the challenge who could unnecessarily change the most numbers in a single simulation file? A minimum allowable temperature of 500K is just nonsense. It's just the temperature value at which the temperature will be cut when it tends to go lower than that. It has no impact when your temperature will not drop below the default value for min allowable temperature of 100K. But assuming, the temperature would drop to let's say 50K, that's just unphysical and should be investigated (air would be liquid at this temperatures). With the default value, you would get a warning message. With your value, you don't get a warning message and therefore you don't know you can't trust your results as they are unrealistic. 

October 16, 2011, 10:58 

#4 
New Member
Andrew Muharib
Join Date: Aug 2011
Posts: 3
Rep Power: 7 
Thank you for your reply Abdul,
I should have probably been more specific about the model I am trying to simulate. Essentially I am attempting to model a heat exchanger of the dimensions shown in a previous figure. The main parameters I want to model are the pressure, pressure coefficient, nusselt number, dimensionless wall distance  around the central tube, as well as being able to view these parameters and vorticity, turbulent kinetic energy instantaneous temperature and velocity as scalar plots. The main idea was to include periodicity across all 3 planes in order to simulate multiple tubes and show the flow in a fully developed simulation. Is there a better method of doing this? I am unsure that my initial method will work, as there will be a transfer of gas across all periodic 3 boundaries defined. The values were changed in order to mimic values that I was given, as I am essentially attempting to validate work already undertaken by a PhD student  this is my current postgrad project. Therefore I need to use most of the values I have previously suggested I appreciate what you have suggested about the mininmum temperature value, and will adjust accordingly. As I was new to CFD modelling I just took it as an arbitrary value. Currently I can simulate the pressure changes, however I get no change in temperature of the flow and a zero value nusselt number  which is clearly incorrect for what I am trying to simulate. I have included another diagram of what I am trying to simulate  thank you very much, your help is greatly appreciated. 

October 22, 2011, 23:54 

#5 
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
Sorry for the late response, I was very busy in the last time and totally forgot to reply.
I think my first shot would have been to use a Symmetry Plane for at least the Z boundary, maybe also for the Y boundary. But I DO NOT want to say, you will get better results. It's just to keep it simple for the first step, later you can check how to get the better results. It's not surprising to get a zero Nusselt number with a zero heat flux. So the main question is: Why is there no heat flux? I would like you to check three things and tell me the outcome:  What happens when you get rid of all periodic interfaces and run it with a velocity inlet / pressure outlet instead?  What thermal specification did you apply to the pipes?  Which temperature do you get in your flow field and what was the initial value? Does it stabilize at a value different to the initialization value or doesn't it change at all? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Use of kepsilon and komega Models  Jade M  Main CFD Forum  24  May 9, 2017 01:53 
Continuing User Defined Real Gas Model issues  aeroman  FLUENT  6  April 8, 2016 03:34 
Wrong calculation of nut in the kOmegaSST turbulence model  FelixL  OpenFOAM Bugs  27  March 27, 2012 09:02 
Low Reynolds kepsilon model  YJZ  ANSYS  1  August 20, 2010 13:57 
2 stage axial turbine model convergence issues  sherifkadry  CFX  2  September 7, 2009 20:51 