[ROY4]

Originally Posted by ghorrocks

1) Your text implies that it is not converging at the start of the simulation, even when you start with quite a small time step. If you need a time accurate simulation you need to fix this - improve mesh quality, use double precision numerics, use a better initial condition, use an even smaller time step. If you are not looking for a completely time accurate simulation then you can ignore this initial lack of convergence as long as it converges later on.

1b) To get an increasing time step you need to converge in 1 or 2 coeff loops, as simple as that.

2) It does not matter which you do first. Convergence criteria is usually the easiest and is only weakly coupled to the others in most cases, so it is a good one to do first. But mesh and time step are coupled together, so when you change one you will change the other. This means sensitivity studies can be iterative.

3) Larger mesh will usually give you a larger time step. But you can only use larger mesh and/or time step if the sensitivity analysis says it is OK for your case.

Dear Glenn,
a) Actually In my case which is a two phase bubble column, finer grid causes errors and we would like to use a larger grid in order to eliminate turbulence modes. So I don't want to make the mesh finer.
b) I used double precision too and overflow was still seen.
c) My boundary condition are just as suggested in most of simulations, since
c-a) I'm using a perforated plate. In this case, using velocity inlet for the small sparger holes, will decrease the quality of the prediction near the saprger. Due to this reason I use source points for air inlet.
c-b)The outlet is degassing which is a designed Boundary condition for bubble column reactors,
c-c) The other boundary is the wall of the column.

d) I used smaller timestep and it diverged very soon.

about your last sentence,
If you are not looking for a completely time accurate simulation then you can ignore this initial lack of convergence as long as it converges later on.

when I was using timestep of 0.05 without time accurate solution in every time step:
The mass conservation is OK and Min=Mout.
The values that I'm going to report as results, are time averaged ones and in fact I validated gas holdup almost accurately and axial liquid velocity with errors especially for H/D>3. But the biggest problem is the turbulent kinetic energy which does not validate at all. actually it is 10 order larger than the experiments.
Then, I thought that maybe the fact that my solution does not get time accurate in every time step causes the turbulent kinetic energy's wrong prediction. So I decided to make it converged and then I understood that my time step might not be small enough. In other words, the solution must get time accurate during 5 iterations at most, and if it doesn't, then the time step that you are using is not small enough (correct me if I'm wrong) so adaptive timestep plays an important role since it can help to find the best time step.
1)any way, should I ignore this Kinetic energy and consider gas holdup and Axial liquid velocity enough for validation?
2) should I keep using 0.05 and do a time independence study for 0.1 and 0.025 as well?

Sorry if I wrote too much. I just wanted to explain the whole adventure.
Thank you

[ghorrocks]

a) Sure, but is your mesh fine enough to be numerically accurate enough for your purposes? You do a sensitivity analysis to work this out.

b) OK, and don't forget improved mesh quality and better initial conditions.

c) OK

d) This suggests your simulation has low numerical stability. Improving mesh quality is the most general improvement to be made in this case.

1) If you do not care about the TKE then you can ignore it, it sounds like the parameters you do care about are accurate enough. If you do care about TKE then you better fix it.

2) It sounds like these simulations are not capturing the startup transient accurately, but it also sounds like you don't care about the startup transient. In that case then don't worry about some non-convergence in the initial time steps, and yes, you should try 0.1 and 0.025 sec time steps for a time step sensitivity analysis.

[ROY4]

Originally Posted by ghorrocks

a) Sure, but is your mesh fine enough to be numerically accurate enough for your purposes? You do a sensitivity analysis to work this out.

b) OK, and don't forget improved mesh quality and better initial conditions.

c) OK

d) This suggests your simulation has low numerical stability. Improving mesh quality is the most general improvement to be made in this case.

1) If you do not care about the TKE then you can ignore it, it sounds like the parameters you do care about are accurate enough. If you do care about TKE then you better fix it.

2) It sounds like these simulations are not capturing the startup transient accurately, but it also sounds like you don't care about the startup transient. In that case then don't worry about some non-convergence in the initial time steps, and yes, you should try 0.1 and 0.025 sec time steps for a time step sensitivity analysis.

Dear Glenn
This is my grid quality:
Minimum Orthogonal Quality = 7.09228e-01
(Orthogonal Quality ranges from 0 to 1, where values close to 0 correspond to low quality.)

Maximum Ortho Skew = 1.94032e-01
(Ortho Skew ranges from 0 to 1, where values close to 1 correspond to low quality.)

Maximum Aspect Ratio = 1.39503e+01
Which I took using Fluent. It all seemed fine.

1) some papers (such as the paper that I'm gonna validate) did report the TKE. So I thought that maybe I need to report it as well. but every other thing in this simulation seems fine enough such as mass conservation as I mentioned.

2) the main problem is that I don't know if this convergence happens in the next timesteps or not? I mean as you said if the non-time accurate time step is only happening in initial timesteps its Ok. but if they keep happening in the next timesteps, they will increase round off errors. which might be a reason for why my RMS residuals are so much chaotic. is there anyway I can understand if my solution is converged in bigger time steps or not?

3) Can I run my simulation with large time step and then make it smaller to get a more accurate result?

4)should I care about the Courant Number or Not?

5) If I run my solution for 0.1, 0.05 and 0.025 and it does not change, Can I say that the simulation is time independence? If yes, then what type of parameter should be compared for time independence study; a parameter in the last time step or a time averaged parameter?

Thank you

[ghorrocks]

Different simulations have different sensitivities to mesh quality. So I cannot assess whether your mesh quality is a problem or not. But I will guarantee that if you improve mesh quality, at least in the region of high residuals, then the simulation will converge faster and more reliably. Time spent improving mesh quality is never wasted.

1) Don't forget that many other factors contribute as well. For instance the choice of turbulence model is likely to have a big effect.

2) For most simulations the residuals are the best judge of convergence. That is why they are the default setting.

3) I don't know what you are modelling so cannot answer that.

4) No. Obtaining a time step size which you show has converged to an accuracy you are happy with is more important for an implicit solver like CFX.

5) Yes. The parameter you compare should be a parameter of interest to you, preferably as a simple number such as pressure loss form inlet to outlet, flow velocity at a point, volume fraction at the outlet.

[ROY4]

Originally Posted by ghorrocks

Different simulations have different sensitivities to mesh quality. So I cannot assess whether your mesh quality is a problem or not. But I will guarantee that if you improve mesh quality, at least in the region of high residuals, then the simulation will converge faster and more reliably. Time spent improving mesh quality is never wasted.

1) Don't forget that many other factors contribute as well. For instance the choice of turbulence model is likely to have a big effect.

2) For most simulations the residuals are the best judge of convergence. That is why they are the default setting.

3) I don't know what you are modelling so cannot answer that.

4) No. Obtaining a time step size which you show has converged to an accuracy you are happy with is more important for an implicit solver like CFX.

5) Yes. The parameter you compare should be a parameter of interest to you, preferably as a simple number such as pressure loss form inlet to outlet, flow velocity at a point, volume fraction at the outlet.

Dear Glenn,

1) I'm using k-epsilon model. As other papers have reported, this model over-predicts TKE. And some other papers that have compared experimental TKE with numerical TKE(using k-epsilon model), has also reported over predicted values. My problem is that my simulation over-predicts it even more than those numerical solutions although I'm using their settings with only some differences such as drag model and lift coefficient. According to what I said, should I report the TKE?

2) That is true, but as my solution is continued and the time is increased, my solution still iterates the maximum coefficient loop in every time step (in all time steps it goes all 5 iterations completely). This means that it has not been time accurate even in higher time steps. Would that be fine or is that a serious problem?

3) I'm working on two phase bubble column (air-water) with Eulerian approach.

4) very good, since when I calculate the Courant number on some planes, their value is sometimes so much high. If Courant is not a matter of concern then I can ignore these high Courant values.

5) So, as I understood till now:
5-a) IF I compare the results of 3 grid sizes (coarse, medium and fine) and my final results do not change;
5-b) IF I compare 3 time steps (such as 0.1, 0.05 and 0.025) and the results remain unchanged (even if my solution did not get time accurate in last time steps)
then I have done my verification and validation. Is that True?

Thank you.

[ghorrocks]

1) That is your decision. You have to judge whether the result is significant or not.

2) We have already discussed this. If a time step does not converge then you risk inaccurate results. But if the inaccurate results occur in a time when you don't care too much about it (eg start-up transient) then it is acceptable as long as it returns to convergence later on.

3) My comment was because I do not know what results you are intending to get out of this simulation, how accurate you need to be, whether the start up transient is important and so on. Why this simulation is being done is important.

5) Yes. This is a very simple check and is good enough for most people. There are more sophisticated approaches available if you want, such as http://journaltool.asme.org/Template...umAccuracy.pdf

[ROY4]

Originally Posted by ghorrocks

1) That is your decision. You have to judge whether the result is significant or not.

2) We have already discussed this. If a time step does not converge then you risk inaccurate results. But if the inaccurate results occur in a time when you don't care too much about it (eg start-up transient) then it is acceptable as long as it returns to convergence later on.

3) My comment was because I do not know what results you are intending to get out of this simulation, how accurate you need to be, whether the start up transient is important and so on. Why this simulation is being done is important.

5) Yes. This is a very simple check and is good enough for most people. There are more sophisticated approaches available if you want, such as http://journaltool.asme.org/Template...umAccuracy.pdf

Dear Glenn,
Thanks for your complete and fast answer.
1) Yes, since I have seen other papers pointed to the TKE over-prediction and my model is somehow difference (such as drag and lift models) which can be another reason for TKE over-prediction, then I feel I report them in my thesis and point to the reasons that might cause this.

2) I checked several papers and a thesis. all of them have used time averaged gas holdup and axial liquid velocity for grid verification (although I could not find any plot for time step study). But now I feel that If my time averaged results are not changing due to grid size or time step change, even If the solution did not get converged in every time step, then I can assume that my solution is acceptable since all parameters I have checked for this subject use time averaged data. Is that True?

3) I feel that since being so much sensitive about modeling this problem has a huge computational cost, most of papers do not risk about using very fine grids or timesteps(At least in most papers I have checked). Also the time averaged results are always reported. Unless some huge computers and processors are valid which in my case is not.

4) So I will try this and Go on.

Thank you so much

[ghorrocks]

1) That sounds a good approach for a research project.

2) A few points here:
2a) Make sure you distinguish between start up transients, when the bubbles first start appearing and the flow is rapidly evolving from the initial condition to the pseudo-steady state condition where the device has been operating for a while. It might not have got to a steady state condition (in fact frequently there is no steady state condition), but the device has got to a condition where a time average of the result is meaningful to represent device performance.

It is likely the other researchers are reporting on the pseudo-steady state results. In this case you do not want to include the start up transient in the time average. It also means that how you get to the pseudo-steady state result is not important as long as you are accurate went you have achieved it. This is why some unconverged time steps during the start up transient is not important.

2b) If your simulation is showing grid and time step independence then you have some confidence that those parameters are accurately set. But if you are still getting some unconverged time steps but your results are accurate anyway - then you need to consider whether your convergence criteria is too tight.

3) CFD is one of the most computer intensive fields in the world today. Many of the world's supercomputers are designed for use for CFD. So you should expect that when you try to properly validate CFD simulations you are going to end up with big meshes and long run times.

If other researchers do it with coarse meshes then consider - did they cut corners and not properly validate their results? In other words is their results inaccurate? Or have they done something in their model which allows them to be accurate on a coarser mesh?

[ROY4]

Originally Posted by ghorrocks

1) That sounds a good approach for a research project.

2) A few points here:
2a) Make sure you distinguish between start up transients, when the bubbles first start appearing and the flow is rapidly evolving from the initial condition to the pseudo-steady state condition where the device has been operating for a while. It might not have got to a steady state condition (in fact frequently there is no steady state condition), but the device has got to a condition where a time average of the result is meaningful to represent device performance.

It is likely the other researchers are reporting on the pseudo-steady state results. In this case you do not want to include the start up transient in the time average. It also means that how you get to the pseudo-steady state result is not important as long as you are accurate went you have achieved it. This is why some unconverged time steps during the start up transient is not important.

2b) If your simulation is showing grid and time step independence then you have some confidence that those parameters are accurately set. But if you are still getting some unconverged time steps but your results are accurate anyway - then you need to consider whether your convergence criteria is too tight.

3) CFD is one of the most computer intensive fields in the world today. Many of the world's supercomputers are designed for use for CFD. So you should expect that when you try to properly validate CFD simulations you are going to end up with big meshes and long run times.

If other researchers do it with coarse meshes then consider - did they cut corners and not properly validate their results? In other words is their results inaccurate? Or have they done something in their model which allows them to be accurate on a coarser mesh?

Dear Glenn,
2a) Do you mean that I should start Time averaging after running my case for some transient time steps? So that I pass the initial time steps?
I feel I still have some problems with understanding this convergence from CFX.

In Fluent, for unsteady solution, we set a total time and a time step and number of iterations for each time step, also a residual criteria. then when we start running our problem, for some first timesteps the solution might complete the whole 40 iterations but in the further timesteps these defined iterations might decrease (for example the 40 initial iterations per timestep will reduce to 20 iterations).

In CFX, we also consider a total time and time step, a convergence criteria and Max/Min coeff. loops(which is the number of the Iterations) But 3-5 number of the coefficient loops in CFX is enough. The type of the residuals that CFX plots (RMS and Max) are different from those that Fluent plots. So I can not see what I see in Fluent here. I mean I can not see iterations of a time step and their convergency (becoming flat) in the console. The only way I can understand If my solution Is becoming flat during these 5 iterations is by checking the number of the iterations that are filled during every time step. In my case, I simulate for a total time of 1000 s and the time step of 0.05. And all of the timesteps from the first time step to the last one, all the 5 iterations are completely spend in the solution.

So I think that my solution does not get Time accurate in any of the timesteps since all 5 iterations are getting complete.

However my final result(the time averaged one that I've checked) is not changing.
Is that enough for simulation? Can I only consider This time-averaged results with out considering the problem I mentioned?
Thank you

[ROY4]

Originally Posted by ROY4

Dear Glenn,
2a) Do you mean that I should start Time averaging after running my case for some transient time steps? So that I pass the initial time steps?
I feel I still have some problems with understanding this convergence from CFX.

In Fluent, for unsteady solution, we set a total time and a time step and number of iterations for each time step, also a residual criteria. then when we start running our problem, for some first timesteps the solution might complete the whole 40 iterations but in the further timesteps these defined iterations might decrease (for example the 40 initial iterations per timestep will reduce to 20 iterations).

In CFX, we also consider a total time and time step, a convergence criteria and Max/Min coeff. loops(which is the number of the Iterations) But 3-5 number of the coefficient loops in CFX is enough. The type of the residuals that CFX plots (RMS and Max) are different from those that Fluent plots. So I can not see what I see in Fluent here. I mean I can not see iterations of a time step and their convergency (becoming flat) in the console. The only way I can understand If my solution Is becoming flat during these 5 iterations is by checking the number of the iterations that are filled during every time step. In my case, I simulate for a total time of 1000 s and the time step of 0.05. And all of the timesteps from the first time step to the last one, all the 5 iterations are completely spend in the solution.

So I think that my solution does not get Time accurate in any of the timesteps since all 5 iterations are getting complete.

However my final result(the time averaged one that I've checked) is not changing.
Is that enough for simulation? Can I only consider This time-averaged results with out considering the problem I mentioned?
Thank you

look at this attached picture;
In the 6th iteration, the residuals are under 1e-4 which is the desired convergence criteria. But the solution does not end at this time step and continues all 10 iterations. after that it begins the next time step and again fills all 10 iterations.
Why is that happening?
I'm really confused.

[ghorrocks]

Convergence Criteria: You probably defined imbalances as an additional convergence criteria, or maybe some other convergence criteria. That additional criteria has not converged so it continues despite the residuals being converged.

2a) Again, I do not know the details of what you are modelling so cannot answer for sure. But from what I guess of your application it is the psuedo-steady state result which is of interest, not the start up transient. So you should only be averaging the psuedo-steady state section for the time averaged result, not the start up transient.

2c) You say you converge in Fluent until the residuals go flat - this sounds like wasted effort to me. It suggests you are gaining little by doing the additional iterations. Might as well do less iterations and be just about as accurate.

[ROY4]

Originally Posted by ghorrocks

Convergence Criteria: You probably defined imbalances as an additional convergence criteria, or maybe some other convergence criteria. That additional criteria has not converged so it continues despite the residuals being converged.

2a) Again, I do not know the details of what you are modelling so cannot answer for sure. But from what I guess of your application it is the psuedo-steady state result which is of interest, not the start up transient. So you should only be averaging the psuedo-steady state section for the time averaged result, not the start up transient.

2c) You say you converge in Fluent until the residuals go flat - this sounds like wasted effort to me. It suggests you are gaining little by doing the additional iterations. Might as well do less iterations and be just about as accurate.

Dear Glenn,
All the settings I have made is like the attached picture, Is there any thing wrong with this?

I checked my linear Solution which is dependent to conservation target and I used its default value(0.01) but in simulation it does not get to this value and is higher such as :6e-1.

2b) yes, I do not start time averaging from the first time step but I start it after 50 seconds of total time. In all references, if for example they run the simulation for 1400 seconds of total time, they time average the results over the last 1300 seconds.

2c) Yes, as soon as in fluent the residuals get to the defined value and does not change, it is said that they are time accurate and the next timestep starts.
My residuals fall under my convergence criteria after 6 iterations but it still keep running the total iterations (max coeff. loop) until it gets to the next time step. May it be due to this reason that I set conservation target to 0.01 But my linear solution does not fall under this value after 10 iterations? (attached picture)
because as you can see in 2nd attached picture, in the 10th iterations all residuals are under 1e-4 (conservation criteria) except the linear solution which is larger than 1e-2.
Even the RMS and MAX Courant number remain constant in every time step.

Thank you

[ghorrocks]

There is nothing wrong with your settings. But whether they are correct is another question. For instance:
* Use are using upwind differencing. This is not recommended.
* You are using second order time differencing. Using second order time differencing while using first order space differencing (upwinding) seems odd.
* You are including the imbalances in your convergence criteria, as anticipated. This shows it is not the residuals which is controlling convergence, but the imbalances. So you should do the sensitivity check on imbalances, not residuals.

The linear solver is different. If the residuals are converging (and yours are) then the linear solver is fine.

[ROY4]

Originally Posted by ghorrocks

There is nothing wrong with your settings. But whether they are correct is another question. For instance:
* Use are using upwind differencing. This is not recommended.
* You are using second order time differencing. Using second order time differencing while using first order space differencing (upwinding) seems odd.
* You are including the imbalances in your convergence criteria, as anticipated. This shows it is not the residuals which is controlling convergence, but the imbalances. So you should do the sensitivity check on imbalances, not residuals.

The linear solver is different. If the residuals are converging (and yours are) then the linear solver is fine.

Dear Glenn,

I have let the default settings of CFX-Pre and did not change any of them.
1) What do you recommend for any of these:
Advection scheme, Transient Scheme and Turbulence numerical?

2) Where did I include the imbalances in my simulation? You mean the Conservation Target? Cause in this link:
https://www.researchgate.net/post/ho...n_in_Ansys_CFX
I read that conservation Target decides for linear solver.
3) Should I stop using conservation target?
4) Is it wrong to include imbalances in the solution?

Thank you

[ghorrocks]

Recommendations unless you have a good reason to do otherwise:
Advection Scheme: HiRes
Transient Scheme: If you are capturing important transient features then second order. If there are transient features present but you are not concerned about capturing the details then first order.
Turbulence Numerical: definitely first order for a multiphase flow. Be aware many simplifications are made in the turbulence model for multiphase flows so you are kidding yourself if you think second order turbulence numerics is more accurate than first for a turbulent multiphase flow.

Your link is wrong. The conservation target does not control the linear solver. It controls the global imbalances of mass, momentum, heat, volume fraction and any other equation present.

Whether you need to use the conservation target depends simulation to simulation. Do a sensitivity study and see if it makes a difference in your case. But don't forget that all it does is impose an additional criteria before a time step is declared converged, which means it may or may not result in additional iterations in a time step.