CFX Parameters Settings
Hi all,
With reference to my previous post,i have decided to work with volumetric heat source. My current aim is to model a 150m tunnel with cross section area 10m wide and 8m high with a volumetric heat source of 3m x 3m x1m high. The picture attached below is already in the symmetry of the actual geometry. And the area circle in pink is half of the volumetric heat source. http://img403.imageshack.us/img403/9963/61361433.th.jpg http://img181.imageshack.us/img181/2182/93920633.th.jpg My aim is to simulate the heat transfer of 4.5MW from the volumetric heat source to the rest of the rest of the fluid surrounding it vie convection n radiation and plot a temperature vs time chart. I tried running my simulation with some initial setting but it seems that there is no heat transfer. Kindly advice if i have make a mistake in my meshing or input settings. Output file is at Post 2. Advice and help is much appreciated. Thanks in advance. http://yfrog.com/b761361433j 
Output File as below:
http://img708.imageshack.us/img708/1636/35135586.th.jpg The simulation is to be carried out under natural convection. I only have the heat release rate as information with zero info on the pressure/mass flow rate etc at both ends of the tunnels. Might be my lack of understanding but i have read through the tutorial that setting Total Pressure @ Inlet and a Velocity/Mass Flow outlet would be a more robust option. Compared to using Total Pressure of 0 Pa and static Pressure of 0 Pa at outlet which is sensitive to initial guess. Thus i have set a 5m/s velocity at the outlet with respect to the axis coordinate. LIBRARY: MATERIAL: Air Ideal Gas Material Description = Air Ideal Gas (constant Cp) Material Group = Air Data, Calorically Perfect Ideal Gases Option = Pure Substance Thermodynamic State = Gas PROPERTIES: Option = General Material EQUATION OF STATE: Molar Mass = 28.96 [kg kmol^1] Option = Ideal Gas END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 1.0044E+03 [J kg^1 K^1] Specific Heat Type = Constant Pressure END REFERENCE STATE: Option = Specified Point Reference Pressure = 1 [atm] Reference Specific Enthalpy = 0. [J/kg] Reference Specific Entropy = 0. [J/kg/K] Reference Temperature = 25 [C] END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.831E05 [kg m^1 s^1] Option = Value END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E2 [W m^1 K^1] END ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^1] Option = Value END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END END END END FLOW: Convection SOLUTION UNITS: Angle Units = [rad] Length Units = [m] Mass Units = [kg] Solid Angle Units = [sr] Temperature Units = [K] Time Units = [s] END ANALYSIS TYPE: Option = Transient EXTERNAL SOLVER COUPLING: Option = None END INITIAL TIME: Option = Automatic with Value Time = 0 [s] END TIME DURATION: Option = Total Time Total Time = 80 [min] END TIME STEPS: Option = Timesteps Timesteps = 1 [s] END END DOMAIN: Fluid Coord Frame = Coord 0 Domain Type = Fluid Location = Fluid BOUNDARY: Inlet Boundary Type = INLET Location = Inlet BOUNDARY CONDITIONS: FLOW DIRECTION: Option = Normal to Boundary Condition END FLOW REGIME: Option = Subsonic END HEAT TRANSFER: Option = Static Temperature Static Temperature = 300 [K] END MASS AND MOMENTUM: Option = Total Pressure Relative Pressure = 0 [Pa] END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END END BOUNDARY: Outlet Boundary Type = OUTLET Location = Outlet BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Cartesian Velocity Components U = 5 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END END END BOUNDARY: Symmetry Boundary Type = SYMMETRY Location = Symmetry XYPlane END BOUNDARY: Walls Boundary Type = WALL Location = Walls BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END MASS AND MOMENTUM: Option = No Slip Wall END WALL ROUGHNESS: Option = Smooth Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Density = 1.2 [kg m^3] Gravity X Component = 0 [m s^2] Gravity Y Component = 9.81 [m s^2] Gravity Z Component = 0 [m s^2] Option = Buoyant BUOYANCY REFERENCE LOCATION: Option = Automatic END END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END FLUID DEFINITION: Fluid 1 Material = Air Ideal Gas Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Option = Thermal Energy END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = k epsilon BUOYANCY TURBULENCE: Option = None END END TURBULENT WALL FUNCTIONS: Option = Scalable END END SUBDOMAIN: Firesource Coord Frame = Coord 0 Location = B161 SOURCES: EQUATION SOURCE: energy Option = Source Source = 4500 [W m^3] END END END END INITIALISATION: Option = Automatic INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic with Value U = 0 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END STATIC PRESSURE: Option = Automatic with Value Relative Pressure = 0 [Pa] END TEMPERATURE: Option = Automatic with Value Temperature = 300 [K] END TURBULENCE INITIAL CONDITIONS: Option = Medium Intensity and Eddy Viscosity Ratio END END END OUTPUT CONTROL: RESULTS: File Compression Level = Default Option = Standard END TRANSIENT RESULTS: Transient Results 1 File Compression Level = Default Option = Standard OUTPUT FREQUENCY: Option = Time Interval Time Interval = 10 [s] END END TRANSIENT STATISTICS: Transient Statistics 1 Option = Arithmetic Average Output Variables List = Temperature END END SOLVER CONTROL: Turbulence Numerics = First Order ADVECTION SCHEME: Option = High Resolution END CONVERGENCE CONTROL: Maximum Number of Coefficient Loops = 3 Minimum Number of Coefficient Loops = 1 Timescale Control = Coefficient Loops END CONVERGENCE CRITERIA: Residual Target = 1.E4 Residual Type = RMS END TRANSIENT SCHEME: Option = Second Order Backward Euler TIMESTEP INITIALISATION: Option = Automatic END END END END COMMAND FILE: Version = 12.0.1 Results Version = 12.0 END SIMULATION CONTROL: CONFIGURATION CONTROL: CONFIGURATION: Configuration 1 Flow Name = Convection END END EXECUTION CONTROL: EXECUTABLE SELECTION: Double Precision = Off END INTERPOLATOR STEP CONTROL: Runtime Priority = Standard MEMORY CONTROL: Memory Allocation Factor = 1.0 END END PARALLEL HOST LIBRARY: HOST DEFINITION: PC Remote Host Name = AdminPC Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX Host Architecture String = winntamd64 END END PARTITIONER STEP CONTROL: Multidomain Option = Independent Partitioning Runtime Priority = Standard EXECUTABLE SELECTION: Use Large Problem Partitioner = Off END MEMORY CONTROL: Memory Allocation Factor = 1.0 END PARTITIONING TYPE: MeTiS Type = kway Option = MeTiS Partition Size Rule = Automatic END END RUN DEFINITION: Solver Input File = C:\Documents\Oct 14th [ Inc FS \ Geometry ]  19th Oct \ Tweaking_4448_Working\dp0\CFX1\CFX\Work1\CFX_002\Configuration1.cfg Run Mode = Full END SOLVER STEP CONTROL: Runtime Priority = Standard MEMORY CONTROL: Memory Allocation Factor = 1.5 END PARALLEL ENVIRONMENT: Number of Processes = 1 Start Method = Serial END END END END 
I can see a few errors.
1) You have set the domain to be "Thermal Energy". This models a heat equation but you will want "Total Energy" to allow the gas to have variable density. 2) You are using the ke turbulence model. SST is probably better. 3) If you want 4.5MW from your heat source your source term is wrong. You have defined it as 4.5MW/m^3 and the source volume is 9m^3 so you will get 40.5MW. 4) You have set max coeff loops to 3 and min to 1. I would remove the minimum and put maybe 10 for the max. Then you adjust the timestep size so you get 35 coeff loops per iteration. Or even better use adaptive timestepping to find it for you. 5) You obviously still need to do a convergence and time step size sensitivity check. Once things are working you need to do this. 
Quote:
Thanks ghorrocks for your advice. 1)My initial choice for Thermal Energy is because from the help file it states the difference between both choice is the negligible in K.E. Your explanation makes things simpler. 2) From my journal which i am referencing, they seems to be using standard K epsilon method. Will try out both and compare the results. *SST seems unable to produce a result and my simulation crash. Might be due to my lack of knowledge or some other issue. Will look into that. 3) My bad, i should not have miss the units. 4) Pardon me as i have left out some parameter i am taking reference from. The journal which i am referencing has provided a simulation time of 80min with a time step of 1s. I have since read up on the adaptive timestepping which you recommended. Will run another simulation for comparison. 5) I don't quiet understand the part on convergence. As for the time step time step size sensitivity check, it is to compliment the adaptive timestepping method to check for the optimal results? There is one more thing i would like to clarify. For output Control>Trn Results>Output Frequency The time interval set would be the amount of backup files created? Setting it as 1s for my 80min simulation would likely to take up a lot of storage space. Pls let me know if i might have interpreted any of the above wrong. Thanks once again for the valuable advice. :) 
1) The thermal energy option means constant density. Buoyancy can be modelled using the bousinesq approximation but that is only accurate for small temperature ranges. My guess is your air will get very hot so you should use the full compressible flow model for better accuracy. Hence my suggestion to use Total Energy option.
2) SST should be as stable as ke. some fiddling should fix this. 4) Adaptive timestepping is good to find appropriate time steps quickly. It is difficult to guess time step size in advance. 5) This is important for all simulations, but if you adaptive timestep to 35 coeff loops then 99% of the time you will be time step convergent. You still need to do the convergence check to ensure you are converging tight enough. (and mesh, and boundary proximity and physics and everything else). More details here: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F 
Quote:
Thanks, appreciate the help a lot. Will read up on the link you provided. :D 
You're only going to get a couple of degrees of heating with those numbers.

Glenn: He is even further off on his power numbers, and much lower than desired. His heat source is 4.5kW/m^3 giving him a total of .0405MW of heat, at least 2 orders of magnitude off his wanted heat source.

Total Energy probably won't hurt, but it's only needed in high speed compressible flows (Mach > 0.25 say). It's not needed in variable density flows when the density variations are due to buoyancy.

Quote:
Quote:
I notice my personal mistake. My intention is suppose to be in MW. I am putting an input of only 4.5 KW. Its tough with less than 6hrs of sleep daily trying out to figure out all this from scratch. Noted the above with thanks. I was just pondering over why did my simulation complete its run with only a little temperature change. Did not wanna post the problem till i get back school to double check my simulation. Thanks a lot guys. :) 
Quote:

Quote:
regarding mesh checking, i have attached a screenshot below. The error is circle in pink. I would assume that this would means that i would have to work on my fluid domain and redefine the mesh further? http://img820.imageshack.us/img820/7381/19083936.jpg ================================================== ====================== As for checking how to check for convergence, boundary proximity and physics i am kinda lost. Just like to verify my understanding. Boundary Proximity: Are you referring to this? http://img513.imageshack.us/img513/976/93657592.jpg The above mention error have occur before. I have read up on the way to remove the error by either changing the outlet to an opening or moving the boundary further down. But if the error is only a single digit which disappear after a few iteration can i safely assume that the it doesn't post a problem towards my solution? ================================================== ====================== http://img51.imageshack.us/img51/4332/32557211.jpg The convergence history for a steady state analysis looks similar to the following http://img2.imageshack.us/img2/5175/80084661.jpg As for convergence, pardon my ability to understand the context of a tighter convergence. With reference to the numbers in pink above. To my understanding this is clearly not a convergence case. I have already done the read up on convergence history Rates less than 1.0 indicate convergence. For a my case of transient analysis. Do i expect the simulation to finally converge? If so then the ideal "Rate" value i would want to expect at the end of my run should be 1 am i right. So for a tighter convergence is to obtain a value below 1 during the run. A higher value such as 0.90.8 would means a slower converge while a lower value signify a faster convergence. But it too fast of a convergence would affect our accuracy of the result? So we are require to "play" around with the initial timestep (adaptive timestepping) and run multi simulations to verify this? The OK and ok by the sides fluctuate during the simulation process, does that calls for an error that i have to take note of or can i brush it all as long as the final iteration ends with all of them showing OK. ================================================== ====================== Finally here are my initial settings for the adaptive timestepping parameters. Is there anything that i have set wrongly or could be optimize? http://img810.imageshack.us/img810/3323/61866650.th.jpg Appreciate help from anyone out there as well. Thanks in advance. 
1) Mesh quality  this is not an error, it just means your poor quality mesh will make it harder to obtain convergence. With a bit of effort you will probably be able to get it to converge, but time spent improving mesh quality is always rewarded with improved simulation time and accuracy.
2) The reverse flow warning is saying you have reverse flow at an outlet. Again, you might be able to get it to converge but you are making things hard for yourself. Move the downstream boundary further downstream so it is beyond the vortex being shed. This is discussed in depth in the documentation. 3) Your convergence on the transient run is very loose on the energy equation. You need to improve that. Your snapshot implies that the adaptive timestepping has hit the minimum time step you set (1s). Make the minimum timestep really small (maybe 1e10s) at let it find whatever timestep it needs to get convergence. The numbers you circle are the convergence rates, not the level of convergence. The RMS residuals and Max residuals tell you the level of convergence you have achieved. 
Quote:
1) Noted. Working on that right now 2) I have gone through the documentation. But by shifting the existing boundary further downsteam, that means that i would need to extending my geometry length? Wouldn't that be affecting my initial geometry design? Thinking deeper into it, i think that would not pose a problem right? Cos it is just providing additional "space". Just need some professional assurance on my above logic. http://img716.imageshack.us/img716/9887/78671571.jpg 3) I have some question for part 3, but i guess i put off till more reading up before i clear up my doubts. Thanks once again. 
Rates less than one indicate that the solution is converging, not that it has converged. You want to look at the RMS and max residuals to judge convergence, as well as imbalances and monitors of bulk quantities (areaAve(Pressure)@<boundary condition>, massFlowAve(Temperature)@<boundary condition>, monitor points, etc.).
As far as the mesh quality check, you are failing the mesh expansion validation on << 1% of elements in the model, which may be perfectly acceptable, depending on whether it's in a region of interest and if there are strong gradients are there. Finally, I would advise you to ignore the artificial wall warning here; the fluid attempts to backflow at startup, probably because you've initialized it with zero flow, but then quickly resolves. If you initialize the problem with the 5 m/s flow you are enforcing, this warning will likely never happen. I would definitely not simply extend the geometry as is, as you would be changing the length of the tunnel. If you feel you need to extend the geometry because the flow field at the outlet is unrealistic, then model a portion of the external atmosphere, for example with a semispherical dome that has an entrainment opening BC. Lastly, I know you said you were enforcing a 5 m/s "wind" through the tunnel. Where did this number come from? Did you pick it out of a hat? This value will strongly affect your results, as the time a fluid parcel spends being heated is inversely proportional to it, so think carefully about it. 
Also, listen to Glenn about the convergence on the energy equation in your transient run. The residuals are high (greater than 1e3 RMS), and recall that the whole purpose of the calculation is the heat transfer. You net to set convergence criteria specifically for the energy equation on the Equation Class Settings tab of the Solver Control. I would also set the Conservation target and create monitor points and monitor expressions to monitor bulk quantities like actual temperatures. Heat transfer calculations are notorious for "converging" on the mass & momentum residuals while bulk quantities are still changing.

Quote:
Hi michael, I have since read up on the way to judge convergence. Referencing the below diagram, the RMS Res is a factor of 10 compared to the Max Res which signify a convergence. http://i54.tinypic.com/11m999d.jpg But ultimately i am still confuse on how to obtain or rather what is a tighter convergence which is mention by ghorrocks. Could you kindly enlighten me on that or point me to a direction where i can do some reading. I may be looking at the wrong direction in the search file. Noted the next 2 paragraph with thanks. Lastly, yes i indeed pull the value of 5m/s out from somewhere. If i am aiming to rely on the heat of the fluid to simulate the flow and rely on convection i should have set it to 0 instead. Thanks michael for the valuable advice. [EDIT] The above analogy made by myself seems to be flawed. By putting a 0 velocity it actually constrain the outward flow of the fluid. Bring about the above error. The 5m/s initial is just a rough guess, intention was to complete the simulation before increasing or reducing the velocity to obtain a similar temperature vs time graph to compare to results of the journal i am taking reference from. 
The RMS residuals being an order of magnitude lower than the maximum residuals does not by itself indicate convergence at all. It seems like you are not really understanding what a "residual" is? It's the fractional change in a solution variable from one iteration to the next. As the residuals approach zero, the solution stops changing with new iterations. When the solution stops changing it has converged. Max residuals are the maximum residual in the mesh for the given equation; RMS is the root mean square of the residuals for the given variable. Generally for adequate convergence in a steady state calculation, you want mass/momentum RMS residuals lower than 10^5. Max residuals will in general be an order of magnitude or so higher.
In CFX pre under the solver control you set the convergence criteria. The default is RMS residuals less than 10^4. This is what Glenn is referring to when he says to tighten the convergence; lower the convergence criteria to a smaller number like 10^5 or 10^6. Also remember that CFX can decide the model is converged because it has met your criteria, but bulk solution quantities can still be changing, or equation imbalances can still be high, etc. 
1 Attachment(s)
http://img513.imageshack.us/img513/835/73538499.jpg
Hi all, need some help to verify my understanding. My knowledge on this is still rather green so please bear with me if my post seems like a repeat of the above advice so correct me if i have interpreted anything wrongly. I have attached the starting portion of the simulation log file on my parameters settings as well. With advice i have set the minimum timestep to be 1E10 w initial timestep at 1E3. With reference to the diagram above, can i safely say that the time step require to start convergence is 1.67777E4. Convergence Criteria Residual Type: RMS Residual Target: 1E05 Conservation Target: Set as 0.01 If the MAX and RMS value at each iteration decrease at individual timesteps it would be still converging. Once the convergence criteria has been reached or the value stop changing, it has converged. So base on which every residual type being set ie. RMS or MAX the simulation would stop after reaching the Residual Target value. [EDIT] The above statement seems wrong. I read through my post and log file and discover that the RMS value goes below 1E05. How do i relate the Residual target value with the RMS and MAX Residual? Quote:
If not the simulation would just end after meeting the Residual Target above. Finally i have attached the start of the simulation log. I seems to have some issue with the simulation with it ending with the below error msg. http://img213.imageshack.us/img213/7577/53038924.jpg Side Question: If according to above i have obtain the timestep before it start converging, can i input the value back to the timesteps options? The method in #02. Or is this a bad idea. TIME DURATION: Option = Total Time Total Time = 80 [min] END TIME STEPS: Option = Timesteps Timesteps = 1.67777E04 
Quote:
Quote:
The residuals can go below your target value on some equations if you have not met your other convergence criteria. You mus meet all convergence criteria for the solver to decide that the job is converged. And again, the solver can meet all your convergence criteria and still not be actually converged if bulk solution quantities like pressure, velocity, temperature are still changing. Quote:
Quote:
Quote:

All times are GMT 4. The time now is 01:02. 