[Danial Q]

Hi everyone,
could anyone please guide me if my transint simulation of Homogeneous multiphase problem involving free surface flow is moving in right direction as It is taking too long (almost its 4 th day ), details are as follows;

Type : transient
Total time : 2e-6s
time step: 5e-10s
initial time = 0s
High resolution and second order backward euler schemes are employed, loops are (3,10), coefficient loop timescale control with RMS (1E-4).

My RMS Courant Number and Max courant Number (both are zero after few initial timesteps), that is real concern. Mesh Expansion factor is also in hundreds(200+).

Thanks

[monkey1]

Hi Danial!
This is a bit too few of information...taking your timestep and iteration loop settings alone i would say 4th day for a max of 40.000 Iterations could be normal depending on:
-How Many CPU's do you use?
-How many Elements does your mesh contain?

Apart from that do you reach your convergence criterion of RMS 1e-4 within the 10 iteration loops? If yes then the first guess is that it is numerically converging. If you always have 10 iteration loops per timestep without reahing rms 1e-4 then it is not converged to its final value for the step. On the other hand courant numbers of 0 juest mean that you have very little changements between 2 time steps.

Other thing that could slow down your calculation is: How often do you write a transient results file and backup files. Do you write out all variables or selected variables? With a hughe mesh this could take some time.

[ghorrocks]

I hope you did a sensitivity analysis on your time step size, mesh size and convergence before starting a 4 day simulation. If you did not do a sensitivity analysis then you have just wasted 4 days as you have no doubt got something wrong and will have to run it again.

[evcelica]

Why such the small timestep size? Courant number of zero too. Not even converging to crappy 1E-4 RMS, I'm no expert, but right off the bat I'm thinking your time steps are way too small. Very small time steps can lead to difficult convergence too.

Glenn, how do you do a sensitivity analysis before running the model?

[Danial Q]

AS far as RMS value is concerned in the beginning of solver, yes it started from 1e-2 and then gained 1e-4 and now after 4 daz it has reached to the value of 1e-8 and yes i m writing transient files after 100 steps,this is mesh details;

Global Statistics :
Global Number of Nodes = 557411
Global Number of Elements = 530304
Total Number of Tetrahedrons = 2101
Total Number of Prisms = 1136
Total Number of Hexahedrons = 521023
Total Number of Pyramids = 6044
Global Number of Faces = 66578
ghorrocks, i did not do sensitivity analysis before running solver but values were same as were previously used in model which i am replicating with same physics.

[ghorrocks]

Glenn, how do you do a sensitivity analysis before running the model?

A typical approach is to just run the first little bit of the simulation, rather than the whole thing. Just run it until something interesting happens. Then do a sensitivity analysis on time step size, mesh and convergence on that initial bit of the simulation. When that is sorted then you do the entire simulation.

[Danial Q]

Could you please comment if it (highlighted Red) is problematic while initial conditions were Vfi (air) =1, Vfi(liq) = 0.


TIME STEP = 1 SIMULATION TIME = 5.0000E-10 CPU SECONDS = 2.376E+01
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 2.376E+01
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.00 | 9.8E-11 | 2.2E-09 | 1.0E+06 F |
| V-Mom-Bulk | 0.00 | 9.7E-11 | 4.1E-09 | 1.0E+06 F |
| W-Mom-Bulk | 0.00 | 2.1E-03 | 2.0E-02 | 1.2E-01 ok|
| Mass-liquid | 0.00 | 1.2E-11 | 5.7E-11 | 0.0E+00 OK|
| Mass-Air at25C | 0.00 | 4.2E-03 | 2.0E-02 | 42.3 7.2E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-liquid | 0.00 | 4.4E-14 | 2.1E-13 | 5.2E-05 OK|
| H-Energy-Air at25C | 0.00 | 1.3E-01 | 6.4E-01 | 3.9E-05 OK|
| T-Energy | 0.00 | 3.5E-04 | 1.7E-03 | 9.4 5.2E-05 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 2 CPU SECONDS = 1.113E+02
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk |99.99 | 7.3E-03 | 2.7E-01 | 1.0E-02 ok|
| V-Mom-Bulk |99.99 | 7.1E-03 | 2.5E-01 | 1.1E-02 ok|
| W-Mom-Bulk |15.11 | 3.1E-02 | 2.6E-01 | 5.1E-03 OK|
| Mass-liquid | 0.54 | 6.5E-12 | 1.6E-10 | 0.0E+00 OK|
| Mass-Air at25C | 0.39 | 1.6E-03 | 7.8E-03 | 42.3 6.9E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-liquid |99.99 | 1.0E-03 | 2.4E-02 | 3.7E-05 OK|
| H-Energy-Air at25C | 0.00 | 4.1E-04 | 9.2E-03 | 2.7E-05 OK|
| T-Energy | 0.00 | 1.3E-06 | 1.0E-05 | 9.4 3.7E-05 OK|
+----------------------+------+---------+---------+------------------+

Is anything unusual in following timestep?? It would be great help if someone could mention it.As i am newbie and it looks fine to me.

TIME STEP = 1430 SIMULATION TIME = 7.1499E-07 CPU SECONDS = 3.326E+05
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 3.326E+05
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 1.00 | 1.4E-09 | 2.8E-08 | 2.7E-03 OK|
| V-Mom-Bulk | 1.00 | 1.5E-09 | 3.7E-08 | 2.6E-03 OK|
| W-Mom-Bulk | 1.00 | 7.6E-09 | 6.0E-08 | 8.0E-04 OK|
| Mass-liquid | 1.15 | 1.2E-13 | 2.6E-11 | 0.0E+00 OK|
| Mass-Air at25C | 1.00 | 1.8E-12 | 3.7E-10 | 27.3 9.3E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-liquid | 1.06 | 1.4E-09 | 1.7E-07 | 5.6E-05 OK|
| H-Energy-Air at25C | 1.00 | 7.4E-05 | 1.9E-04 | 1.3E-05 OK|
| T-Energy | 1.01 | 8.9E-06 | 3.1E-05 | 9.4 5.6E-05 OK|
+----------------------+------+---------+---------+------------------+

Thanks in advance

[ghorrocks]

It is common to have the first coeff loop in a time step have strange residuals, which become more normal in the second loop. This is sometimes a sign of too small a time step. How have you determined your time step size?

The fastest way to find a good time step size is to use adaptive timesteps, converging on 3-5 coeff loops per time step (although 5-10 for complex multiphase models sometimes helps), in combination with a sensible convergence criteria. Also - if this model includes surface tension you will need very small time steps, so aim for the 3-5 goal in that case.

[Danial Q]

Infact, i did not calculate timestep by myself but used the same values which i had as a data from previous model which i am replicating. And yes, my model includes surface tension, phase chnage , free surface and heat transfer so its one of the reasons ,I just used the same old values as smaller timesteps.
its almost 6th day...of solver. I should have used adaptive timestepping scheme.

[Danial Q]

After 8 days of running solver, it just turned out to show some return code error 1, and how can i find error ??? that what possible be the cause of errors? Could you please give some tips???How to find specific error in output file?


Thanks

[ghorrocks]

Unfortunately there is no public list of error codes. You will have to post the section of the output file around the error for us to help. Also post the CCL while you are at it.

[Danial Q]

Here are files (CCl details & Error ) with last few iterations befor error occured. I hope it would be helpful.

Thanks

[ghorrocks]

Your time step is too small. You might need a small time step at the start to get going but you certainly do not need it down the track. Consider using adaptive time steps converging on 3-5 coeff loops per iteration.

Your material properties with step changes is always going to be numerically unstable. This is always going to be difficult (or impossible) to converge.

Do not use expert parameters unless you know you need them.

[Danial Q]

I am wondering if I can change the time step during transient simulation. Or this option is possible wIth adaptive time stepping scheme.
The other thing about materials properties, what could be the other possible options for defining them? While i have to definfe them as Temp. function to make phase change occur.

Thanks

[ghorrocks]

You can define time step to be a function of anything you like through CEL. But as you probably don't know in advance what the best time step size is then why not just use adaptive time stepping and let it sort itself out for itself?

I am well aware that you have defined material properties as functions of temperature to simulate phase change. Again, you can make them functions of just about anything with CEL, but whether you would want to is another question.

[Danial Q]

As far as , changing time step is concerned, I was asking if i can change it during solver run by any means. I will try the adpative timestepping this time, but how to guess, decrease and increase factor or max/min time step? wild guess?

The other thing about material properties, I guess defining as function of temperature in my case is the only solution, looks reasonable to me. What other possibilities, you think are practical to change the phase? Yes, you are right, CEL can be used to define any thing.

Thanks

[ghorrocks]

You have to stop and restart to manually change time step.

For adaptive time stepping use 1e-20 as the minimum, 1e+20 as the maximum. Only restrict it if you have a good reason to do so.

I will not answer your second question as I extensively answered that on a previous thread.

[Danial Q]

I gave max time step value to 1e+20 but ,it showed global error to minimize this value less than total time value which was ofcourse in micro sec.
I asked about the material properties thing because I did not know ,in what context you were saying that. As, you would have seen in Result file that I had defined them as CEL already.

Thanks

[Danial Q]

I used adaptive scheme for time stepping this time and it seems that it worked but accumulated timesteps were just 100 (is'nt it too short for free surface multiphase); . I got a creepy notice which is botheirng me.

" --------------------------------------------------------------------+
| ****** Notice ****** |
| While evaluating |
| liquidNi.Static Entropy |
| on domain "splat", |
| the variable |
| liquidNi.Temperature |
| went outside of its lower limit. Its minimum value was |
| 0.0000E+00[K]. The bounds error was handled by clipping. |
| If this situation persists, consider increasing the table range. |
+--------------------------------------------------------------------+
Should I consider it done while "linear solution" values are OK?? And how can we improve solution even though it seems converged, does setting tight value for residuals work well or decreasing initial timestep would help better??

Thanks

[ghorrocks]

Did not I say right at the start that the approach you are taking was likely to be numerically unstable? Well, this looks like numerical instability to me.