[Flaky]

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.





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.

[Flaky]

Output File as below:


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 = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-2 [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.E-4
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 = Admin-PC
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
Host Architecture String = winnt-amd64
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 = k-way
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\CFX-1\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

[ghorrocks]

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 k-e 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 3-5 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.

[Flaky]

Originally Posted by ghorrocks

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 k-e 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 3-5 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.

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.

[ghorrocks]

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 k-e. 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 3-5 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.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[Flaky]

Originally Posted by ghorrocks

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 k-e. 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 3-5 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.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Thanks, appreciate the help a lot.
Will read up on the link you provided.

[michael_owen]

You're only going to get a couple of degrees of heating with those numbers.

[singer1812]

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.

[stumpy]

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.

[Flaky]

Originally Posted by michael_owen

You're only going to get a couple of degrees of heating with those numbers.

Originally Posted by singer1812

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.

Thanks guys,

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.

[ghorrocks]

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.

Incorrect. When the temperature range becomes large enough the bossinesq assumption looses accuracy. You need the full ideal gas equation so the variable density can be accounted for. It is not a mach number effect.

[Flaky]

Originally Posted by ghorrocks

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 k-e. 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 3-5 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.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Hi ghorrocks,

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?


================================================== ======================

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?

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?

================================================== ======================



The convergence history for a steady state analysis looks similar to the following



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 0.9-0.8 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?



Appreciate help from anyone out there as well.
Thanks in advance.

[ghorrocks]

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 1e-10s) 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.

[Flaky]

Originally Posted by ghorrocks

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 1e-10s) 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.

Hi ghorrocks.

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.




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.

[michael_owen]

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 semi-spherical 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.

[michael_owen]

Also, listen to Glenn about the convergence on the energy equation in your transient run. The residuals are high (greater than 1e-3 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.

[Flaky]

Originally Posted by michael_owen

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 semi-spherical 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.

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.


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.

[michael_owen]

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.

[Flaky]

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 1E-10 w initial timestep at 1E-3. With reference to the diagram above, can i safely say that the time step require to start convergence is 1.67777E-4.

Convergence Criteria
Residual Type: RMS
Residual Target: 1E-05

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 1E-05. How do i relate the Residual target value with the RMS and MAX Residual?

Originally Posted by michael_owen

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.

The above statement is to advice me on setting convergence target, so as to ensure that residual criteria and global balances are met.
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.




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 = 1.67777E-04

[michael_owen]

Originally Posted by Flaky

Once the convergence criteria has been reached or the value stop changing, it has converged.

What values are you refering to? The solution values or the residual values? If the latter stop changing, the solution may not be converged if they are still high. Also, the solution has converged once the convergence criteria have been reached AND imbalances are negligable AND bulk quantities like pressures, velicities and temperatures have stopped changing, not "or".

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 1E-05. How do i relate the Residual target value with the RMS and MAX Residual?

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.

The above statement is to advice me on setting convergence target, so as to ensure that residual criteria and global balances are met.
If not the simulation would just end after meeting the Residual Target above.

Almost, but also, you need to create monitor points and expressions in CFX-Pre to monitor bulk solution quantities and make sure that they are steady, at least for a steady state run. Obviously for a transient run you may have transient effects.

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.

You probably ran out of disk space, or the drive was busy or something.

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 = 1.67777E-04

Sometimes it's a good idea, sometimes it's a bad idea. Do you expect conditions to change such that the required timestep will also change? If so, you should probably not. In your case, it's probably fine.