[ROY4]

Hello everyone
I'm modelling a bubble column. during time independence study, when I decreased the time step from 0.05 to 0.025, after about 3 days of simulation, my run has stopped with the below error:
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 4 CPU SECONDS = 7.741E+05

An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver could not be started, or exited with return |
| code 255: . No results file has been created


+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory E:\Abolfazli\Test 3-0.025 |
| s\Transient\25spargertransient_002: |
| |
| 9800.trn, 9600.trn, 9400.trn, 9200.trn, 9000.trn, 8800.trn, |
| 8600.trn, 8400.trn, 8200.trn, 8000.trn, 7800.trn, 7600.trn, |
| 7400.trn, 7200.trn, 7000.trn, 6800.trn, 6600.trn, 6400.trn, |
| 6200.trn, 6000.trn, 5800.trn, 5600.trn, 5400.trn, 5200.trn, |
| 5000.trn, 28200.trn, 28000.trn, 27800.trn, 27600.trn, 27400.trn, |
| 27200.trn, 27000.trn, 26800.trn, 26600.trn, 26400.trn, 26200.trn, |
| 26000.trn, 25800.trn, 25600.trn, 25400.trn, 25200.trn, 25000.trn, |
| 24800.trn, 24600.trn, 24400.trn, 24200.trn, 24000.trn, 23800.trn, |
| 23600.trn, 23400.trn, 23200.trn, 23000.trn, 22800.trn, 22600.trn, |
| 22400.trn, 22200.trn, 22000.trn, 21800.trn, 21600.trn, 21400.trn, |
| 21200.trn, 21000.trn, 20800.trn, 20600.trn, 20400.trn, 20200.trn, |
| 20000.trn, 19800.trn, 19600.trn, 19400.trn, 19200.trn, 19000.trn, |
| 18800.trn, 18600.trn, 18400.trn, 18200.trn, 18000.trn, 17800.trn, |
| 17600.trn, 17400.trn, 17200.trn, 17000.trn, 16800.trn, 16600.trn, |
| 16400.trn, 16200.trn, 16000.trn, 15800.trn, 15600.trn, 15400.trn, |
| 15200.trn, 15000.trn, 14800.trn, 14600.trn, 14400.trn, 14200.trn, |
| 14000.trn, 13800.trn, 13600.trn, 13400.trn, 13200.trn, 13000.trn, |
| 12800.trn, 12600.trn, 12400.trn, 12200.trn, 12000.trn, 11800.trn, |
| 11600.trn, 11400.trn, 11200.trn, 11000.trn, 10800.trn, 10600.trn, |
| 10400.trn, 10200.trn, 10000.trn |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| E:\Abolfazli\Test 3-0.025 s\Transient\25spargertransient_002: |
| |
| pids, mon |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

Does anyone know what does this 255 error code means?
If it means solution divergence, what can I do to correct it?
the .out file which is created is about 300 Mb. Shall I send it?
by the way can anyone help me to checkout if my setting are all right or not?
If anyone can please let me know to send you my cfx pre settings.
thanks alot

[ghorrocks]

There is no description of what the CFX error numbers mean. I don't know why they bother telling you a error number when they don't give you any information about it. But that is just my whinge.

This looks like the network went down and it crashed your job. When you do long simulations like this you must write full transient results files every now and again so you can recover from this sort of glitch. I trust you did save full transient results files.....

Also this would be a good time to look at your network and check it is reliable, that somebody did not turn something off, and that it is not getting hammered by another user.

[ROY4]

Originally Posted by ghorrocks

There is no description of what the CFX error numbers mean. I don't know why they bother telling you a error number when they don't give you any information about it. But that is just my whinge.

This looks like the network went down and it crashed your job. When you do long simulations like this you must write full transient results files every now and again so you can recover from this sort of glitch. I trust you did save full transient results files.....

Also this would be a good time to look at your network and check it is reliable, that somebody did not turn something off, and that it is not getting hammered by another user.

Dear Glenn,
1) Does it mean that my settings are all right and it has nothing to do with divergence? I attached the .out file too. Did you check that as well?

2) By the way, How can I check courant number? I want to see if my time step is fine..I read that I should calculate it from courant number, but since my case is 2 phase flow, should it be water courant, air courant or total courant?
what about physical time step? should I use that as well? how to calculate it?

3)Finally can you please tell me if I should do grid study and then time study or there are no differences?
thanks

[ghorrocks]

1) I cannot be sure about your settings but it appears to have nothing to do with convergence. I did check your out file.

2) Don't worry about checking your Courant number to see if it is OK. CFX is an implicit solver and is not limited by a specific Courant number like explicit codes are. Instead you should do a time step sensitivity check.

3) You should always do a mesh sensitivity check. It is a bit iterative between mesh and time step - once you have determined one then do the other you have to check the first one again. This iterations can be reduced by using adaptive time stepping homing in on 3-5 coeff loops per iteration and then it automatically finds the time step and you only have to find the right mesh size.

4) An extra one for you: Don't forget convergence criteria. You also need to determine that the convergence criteria you are using is adequate.

[ROY4]

Originally Posted by ghorrocks

1) I cannot be sure about your settings but it appears to have nothing to do with convergence. I did check your out file.

2) Don't worry about checking your Courant number to see if it is OK. CFX is an implicit solver and is not limited by a specific Courant number like explicit codes are. Instead you should do a time step sensitivity check.

3) You should always do a mesh sensitivity check. It is a bit iterative between mesh and time step - once you have determined one then do the other you have to check the first one again. This iterations can be reduced by using adaptive time stepping homing in on 3-5 coeff loops per iteration and then it automatically finds the time step and you only have to find the right mesh size.

4) An extra one for you: Don't forget convergence criteria. You also need to determine that the convergence criteria you are using is adequate.

Dear Glenn,
Thank you so mush, cause I was really worried about the settings and you really advised me helpfully.
only I just want to ask my last questions:
1) the residual RMS plot that I get for this simulation, seems pretty chaotic. Do you think that this is fine or I should have a smoother one?
2) by the way, how many iterations do you suggest for every time step at least? currently i use only 10 iterations for each time step.
thank you

[ghorrocks]

Is this a transient simulation? My previous posts assumed that this is a transient simulation.

If your simulation is steady state then your convergence is a problem. If your simulation is transient then as long as each time step achieves your convergence criteria it is fine.

In transient simulations I recommend 3-5 coeff loops per time step. The easiest way to do this is with adaptive time stepping homing in on 3-5 coeff loops per time step.

[ROY4]

Originally Posted by ghorrocks

Is this a transient simulation? My previous posts assumed that this is a transient simulation.

If your simulation is steady state then your convergence is a problem. If your simulation is transient then as long as each time step achieves your convergence criteria it is fine.

In transient simulations I recommend 3-5 coeff loops per time step. The easiest way to do this is with adaptive time stepping homing in on 3-5 coeff loops per time step.

Dear Glenn,
Yes it is a transient solution. First I ran a steady solution and used it as my initial guess. The image that I attached is transient RMS plot, since this problem is completely unsteady that I assume it will never reach a steady state.

1) to be honest, since yesterday I have studied the CFX guides about adaptive timestep, but I didn't understand what to define for some of these tabs in attached image.. which might be because the explanation does not seem to be enough for me (for example I have no experience on time step decrease/increase factor and timestep update frequency. is first update time OK to be set to zero?). I filled these tabs in the following form(image 2). is this fine or it has a problem?

2) by the way you talked about coefficient loops to be 3-5, I set to 10 since I feel in 3-5 loops it might not get time accurate in that time step. actually in every timestep all 10 iterations are complete which means that in 10 iterations the solution of that time step does not get time accurate.

3) Whats the difference of target Max/Min Loop in adaptive time step with coeff. Loop one in solver control? Does it mean that in adaptive time, target loop will change the time step in for example 3-5 loops to find the proper time step but the coeff. loop means number of iterations in each time step?

THANK YOU

[evcelica]

All that info on adaptive time stepping settings is in the documentation. (and also kind of obvious I thought.)

If solver reaches convergence before min target # of iterations, it increases your time step. If it goes over the max target #, it decreases the time step. Equal to or in between your targets, and the time step stays the same. When it does change the time step, it does so according to the ratios you set for increase and decrease, and up/down to the limits you set.



If it is doing 10 iterations and not converging, that means your time step is too large. Usually after 7-8 iterations convergence doesn't get any better, 10 is definitely wasteful. 3-5 like Glenn says (WITH A SMALLER TIME STEP) will be better.

Also why limit the minimum time step? Just set to 1e-10[s], and let the solver adapt and find where it wants to be for your simulation. Note what the Courant number is (output by solver) for informational purposes.

[ROY4]

Originally Posted by evcelica

All that info on adaptive time stepping settings is in the documentation. (and also kind of obvious I thought.)

If solver reaches convergence before min target # of iterations, it increases your time step. If it goes over the max target #, it decreases the time step. Equal to or in between your targets, and the time step stays the same. When it does change the time step, it does so according to the ratios you set for increase and decrease, and up/down to the limits you set.



If it is doing 10 iterations and not converging, that means your time step is too large. Usually after 7-8 iterations convergence doesn't get any better, 10 is definitely wasteful. 3-5 like Glenn says (WITH A SMALLER TIME STEP) will be better.

Also why limit the minimum time step? Just set to 1e-10[s], and let the solver adapt and find where it wants to be for your simulation. Note what the Courant number is (output by solver) for informational purposes.

Dear Erik
Thanks for your answer, but for me I need to know more about how it works. only reading 2 lines about it is not enough for me because those 2 lines of explanation are guessable by only reading the title of that tab. But how should I know if those values that are set as default of adaptive time are fine enough for my case when I have no experience in using adaptive time step?

2) where is this minimum time step of 1e-10? I did not see any default of this time step in anywhere.

3) Can I minimize the total time if I minimize the time step?
Currently I'm running for 1000 seconds and time step of 0.05 as it was suggested by the paper I'm going to validate.
As I understood from your guides, I must keep number of iterations 5 and instead decrease the time step until it gets converged in those 5 iterations. Is this true if I don't want to use adaptive time step?

4) if the simulation does not get time accurate ( converged) in every time step and starts the next time step, would the solution be wrong?
Thank you

[ROY4]

Originally Posted by ROY4

Dear Erik
Thanks for your answer, but for me I need to know more about how it works. only reading 2 lines about it is not enough for me because those 2 lines of explanation are guessable by only reading the title of that tab. But how should I know if those values that are set as default of adaptive time are fine enough for my case when I have no experience in using adaptive time step?

2) where is this minimum time step of 1e-10? I did not see any default of this time step in anywhere.

3) Can I minimize the total time if I minimize the time step?
Currently I'm running for 1000 seconds and time step of 0.05 as it was suggested by the paper I'm going to validate.
As I understood from your guides, I must keep number of iterations 5 and instead decrease the time step until it gets converged in those 5 iterations. Is this true if I don't want to use adaptive time step?

4) if the simulation does not get time accurate ( converged) in every time step and starts the next time step, would the solution be wrong?
Thank you

**Actually I decreased my time step to 1e-4 and my total time to 500, number of iterations per time step decreased to 2 iterations. The RMS residual plot started to get flat compared to the last cases. Is that OK?
How should I know that my convergence criteria have been met??
The RMS Courant number per time step is also zero.
Please help me with this.

[ghorrocks]

If the residuals graph is less than your convergence criteria then those time steps converged.

You should also be asking if the convergence criteria you defined is adequate, or even if it is too tight.

[ROY4]

Originally Posted by ghorrocks

If the residuals graph is less than your convergence criteria then those time steps converged.

You should also be asking if the convergence criteria you defined is adequate, or even if it is too tight.

Dear Glenn,
1) As I can see the RMS residuals are now under 1e-4. I sent a picture in my last quote. and you can see its below 1E-4 which is my residual target.

2) About the convergence criteria that you asked, I used the default convergence criteria which is 0.01. and my residuals are under 1e-4 which is 2 orders less than convergence criteria. Although I suppose that 0.01 is a bit loose for simulation. isn't that?

3) About the timestep, if I use time step of 1e-4, then for total time of 500 seconds, I will have 5 million timesteps, and since in every time step 2 iterations are solved, it will be 10 million iterations overall. that I assume it has a large computational cost. I would like to ask, now that I have minimized the timestep, can I decrease the total time?

4) By the way, due to the last solutions I made with timestep of 0.05 for 1000 s total time, I could validate my gas holdup almost accurately, axial liquid velocity with error and the turbulent kinetic energy was really wrong (about an order larger than the experimental values). I want to know, are those validations wrong?

Thanks

[ghorrocks]

2) I do not understand what you are saying here. The normal way to work out what convergence criteria you require is to do a sensitivity study. Change the convergence criteria by a factor of 10 (say 1E-3, 1E-4, 1E-5) and compare the results for a parameter you care about. The result should converge to a constant value at tight convergence, so you use the loosest criteria which is accurate enough to a tolerance you are happy with.

3) Yes, transient simulations are very expensive. That is why you need to carefully define the settings to be tight enough to be accurate and loose enough to not take too long. We recommend you use adaptive time stepping so the solver automatically adjusts the time step to the optimum size. The time step you are proposing appears far from optimum, and will result in the simulation taking far longer.

4) You would have to check. You really should read about simulation accuracy and verification - This is the general FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F and this one has a link to an excellent article on how to work out your accuracy: https://www.cfd-online.com/Wiki/Ansy...publishable.3F

[ROY4]

Originally Posted by ghorrocks

2) I do not understand what you are saying here. The normal way to work out what convergence criteria you require is to do a sensitivity study. Change the convergence criteria by a factor of 10 (say 1E-3, 1E-4, 1E-5) and compare the results for a parameter you care about. The result should converge to a constant value at tight convergence, so you use the loosest criteria which is accurate enough to a tolerance you are happy with.

3) Yes, transient simulations are very expensive. That is why you need to carefully define the settings to be tight enough to be accurate and loose enough to not take too long. We recommend you use adaptive time stepping so the solver automatically adjusts the time step to the optimum size. The time step you are proposing appears far from optimum, and will result in the simulation taking far longer.

4) You would have to check. You really should read about simulation accuracy and verification - This is the general FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F and this one has a link to an excellent article on how to work out your accuracy: https://www.cfd-online.com/Wiki/Ansy...publishable.3F

Dear Glenn
thanks for your answer,

2) for my second question I didn't know that convergence criteria needs to be studied as well as time step and grid. So I need to study tighter convergence criteria as well as the default one. right?

3)I like to use the adaptive time step but as I said I don't know how should I fill the empty tabs and unfortunately it seemed that every one see my question so obvious that they did not see it necessary to check if I have set them right or wrong. anyway I attach its picture again so that if you(or anyone else) would please like to help me with that.(?)

4) Thanks for the links You mentioned, I will check them all.

Thank you

[ROY4]

Originally Posted by ROY4

Dear Glenn
thanks for your answer,

2) for my second question I didn't know that convergence criteria needs to be studied as well as time step and grid. So I need to study tighter convergence criteria as well as the default one. right?

3)I like to use the adaptive time step but as I said I don't know how should I fill the empty tabs and unfortunately it seemed that every one see my question so obvious that they did not see it necessary to check if I have set them right or wrong. anyway I attach its picture again so that if you(or anyone else) would please like to help me with that.(?)

4) Thanks for the links You mentioned, I will check them all.

Thank you

bY THE WAY, BECAUSE i HAVE TO USE TIME AVERAGING, IF i USE ADAPTIVE TIME STEP i CAN NOT USE TIME AVERAGING ANYMORE.

[ghorrocks]

2) Yes, the basic things you need to check are set correctly on a transient simulation are the time step size, mesh size and convergence criteria.

3) Try this:
Total Time = 1000[s]
First update = 0[s]
Time step update freq = 1
Initial Time step = 1e-6[s]
Maximum timestep = 0.05 [s]
Minimum time step = 1e-10[s]
target max = 5
target min = 3
decrease factor = 0.8
increase factor = 1.06

The initial time step may be a bit small but it will quickly increase to find the correct size. Just let it run.

5) Time averaging - if you are using the built in time averaging stuff then yes, you should not use adaptive time stepping. But I would run a test run to find what time step it recommends and then do a second simulation using that time step as a fixed time step.

If you are doing your own time averaging - then you can account for the variable time step by including the time step size in your averaging function.

[ROY4]

Originally Posted by ghorrocks

2) Yes, the basic things you need to check are set correctly on a transient simulation are the time step size, mesh size and convergence criteria.

3) Try this:
Total Time = 1000[s]
First update = 0[s]
Time step update freq = 1
Initial Time step = 1e-6[s]
Maximum timestep = 0.05 [s]
Minimum time step = 1e-10[s]
target max = 5
target min = 3
decrease factor = 0.8
increase factor = 1.06

The initial time step may be a bit small but it will quickly increase to find the correct size. Just let it run.

5) Time averaging - if you are using the built in time averaging stuff then yes, you should not use adaptive time stepping. But I would run a test run to find what time step it recommends and then do a second simulation using that time step as a fixed time step.

If you are doing your own time averaging - then you can account for the variable time step by including the time step size in your averaging function.

Dear Glenn,
I used
Total Time = 20[s]
First update = 0[s]
Time step update freq = 1
Initial Time step = 0.05[s]
Maximum timestep = 0.05 [s]
Minimum time step = 1e-7[s]
target max = 5
target min = 3
decrease factor = 0.8
increase factor = 1.06

It decreased Until 8e-5 which I think is a very small timestep.
1) If I make the mesh finer, will the time step increase or not? is there any other way I can increase the time step?
2) If I decrease convergence criteria (e.g. 1e-3), then my time step might reduce even more than this. right?
3) If in the next iterations, bigger timesteps can be used as well, does adaptive time average increase the time step or it will continue the whole simulation with the first proper timestep that has founded?

3) I'm using arithmetic average in Trn Stats (mentioned picture), and I suppose it will not work with an adaptive time step since it needs to be specified as a constant value for up and low limits. But as you said, I can find the proper timestep and run another simulation with the proper one to use this time averaging.
Thank you so much

[ghorrocks]

If you used an initial time step of 0.05[s] and it decreased it to 8e-5[s] then it says your initial time step is way too big. My guess of 1e-6[s] is better as it will converge OK from the first time step and increase the time step until it finds a suitable one. Please note my recommended settings are not guesses - they are likely to be about right as I have been doing this for years. If you try other settings you are probably just wasting your time.

If you make the mesh finer the time step required will get finer. This is why CFD simulations rapidly get so big that they need to run on supercomputers.

If you loosen the convergence criteria then adaptive time stepping will automatically adjust the time step larger for you. But you need to show that the looser convergence criteria is OK for your simulation accuracy before you do this.

Adaptive time stepping will keep adjusting the time step throughout the simulation.

[ROY4]

Originally Posted by ghorrocks

If you used an initial time step of 0.05[s] and it decreased it to 8e-5[s] then it says your initial time step is way too big. My guess of 1e-6[s] is better as it will converge OK from the first time step and increase the time step until it finds a suitable one. Please note my recommended settings are not guesses - they are likely to be about right as I have been doing this for years. If you try other settings you are probably just wasting your time.

If you make the mesh finer the time step required will get finer. This is why CFD simulations rapidly get so big that they need to run on supercomputers.

If you loosen the convergence criteria then adaptive time stepping will automatically adjust the time step larger for you. But you need to show that the looser convergence criteria is OK for your simulation accuracy before you do this.

Adaptive time stepping will keep adjusting the time step throughout the simulation.

Dear Glenn,

1) Actually I though that whether I start from 1e-6 and increase the time step or start from 0.05 and decrease it, I will obtain the same time step. but it is not true.
Actually I set your settings and the timestep decreased to smaller values such as 1e-9. I feel this is worst. I need larger time step size to speed up the solution.
By the way, when I changed the settings to your suggested values, you mentioned that the initial timestep will increase to give me a good time step. but vice versa It decreased and finally stopped with an overflow massage at timestep 5.903e-9. I beg you to help me, its a long time that I'm working on this without getting any appropriate result and my thesis is really dependent on this.

I also read in tutorial that:
(If the actual number of coefficient loops used is less than the Target Minimum Coefficient Loops, the timestep size is increased. If the actual number of coefficient loops used is greater than the Target Maximum Coefficient Loops, the timestep size is decreased)
I have no idea that what can I do to get an increasing time step..

2)As my 2nd question, which one I should do first? Grid study? time study? or convergence criteria study?

3) If I use larger grid size, will it help me to increase the time step? if yes, do you recommend it for me?

Thanks

[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.