[lgtmelo]

Originally Posted by ghorrocks

This FAQ might help now: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

thats where i got the idea of playing with the timestep. do you think i should try the timestep keeping it laminar, or go transient + laminar?

i didnt understand why you mentioned the turbulence models, i thought we were going full laminar now

[ghorrocks]

The comment about the turbulence models was just the explain why it has not gone unstable.

Yes, as the FAQ recommends adjust the time step in a steady state run. If it converges fantastic. But if you cannot get it to converge then go transient.

[lgtmelo]

Originally Posted by ghorrocks

The comment about the turbulence models was just the explain why it has not gone unstable.

Yes, as the FAQ recommends adjust the time step in a steady state run. If it converges fantastic. But if you cannot get it to converge then go transient.

will do and let you know! many thanks

[Gert-Jan]

Originally Posted by lgtmelo

got it. I will run in parallel (another machine) to check it. the bacteria density is of 1100kg/m3, just a bit higher than water. i am using buoyancy (-gravity at vertical axis only).

I think you could switch of buoyancy. Settling of 1mu bacteria is not something that adds to this calculation.

[lgtmelo]

Originally Posted by Gert-Jan

I think you could switch of buoyancy. Settling of 1mu bacteria is not something that adds to this calculation.

good point as well. still running SS laminar, will try this afterwards. thank you

[Gert-Jan]

I would switch it off since it will cost a little extra calculation time, but you won't see any difference in the simulation results. Unless you have creeping flow, but you haven't so......

[lgtmelo]

good morning everyone. quick update: i tried running SS laminar, but I got RMS around 10^-2 and velocity monitor wouldn't stabilize, so as Glenn suggested, I then went transient.


solver is still running under transient. i have the flow as laminar and one-way coupling as we talked about, as well as no buoyancy as suggested above:

================================================== ====================
| Timestepping Information |
----------------------------------------------------------------------
| Timestep | RMS Courant Number | Max Courant Number |
+----------------------+----------------------+----------------------+
| 2.0000E-04 | 0.04 | 0.78 |
----------------------------------------------------------------------

residuals seem very ok to my knowledge:

----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 1.00 | 1.1E-07 | 4.0E-06 | 6.2E-03 OK|
| V-Mom | 1.00 | 1.1E-07 | 4.2E-06 | 6.1E-03 OK|
| W-Mom | 1.00 | 1.2E-07 | 7.1E-06 | 6.6E-03 OK|
| P-Mass | 1.00 | 8.5E-07 | 5.8E-05 | 5.0 8.4E-02 OK|
+----------------------+------+---------+---------+------------------+


and so far, still only 1 paticle being injected:

+--------------------------------------------------------------------+
| Particle type | Fate type Particles |
+--------------------------------------------------------------------+
| BACTERIA | Entered domain : 1 |
| | Continue from last time step : 1220 |
| | Waiting for next time step : 1221 |
+--------------------------------------------------------------------+

some things i still dont understand, when comparing to the steady state i was running: why don't i see particles being captured on walls? is it because I still havent reached this "time" of the run? also, how to I put it in terms like it showed in steady state, where 1000 particles were injected and I was able to know how many were captured on the infill and how many continued to outlet?


other question: for this scenario, is it ok to work with Co > 1 or should I keep it like this? its taking forever. for a 7.5s residence time, with timestep of 10^-4, it will take some more days.

again, very grateful for every help I received so far here.

[ghorrocks]

You don't see particles on walls yet as the particles have not got far enough in the flow to hit the walls. The "Waiting for next time step" count shows all these particles are in the flow and still moving along.

If you are going to do this as transient you are going to have to wait longer.

I would recommend you check whether the poorly converged SS run is still good enough (see the FAQ). It probably is still good enough to use and transient is not required, but you should check.

Don't worry about the Courant number. This is an implicit solver, it does not have a Courant Number restriction.

Why are you using a time step size of 10^-4? If you have not set the time step size with a sensitivity analysis then it is almost certainly wrong. I would recommend you use adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size are wide enough you never hit it, and make the initial time step size the 10^-4 you are currently using.

[lgtmelo]

Originally Posted by ghorrocks

You don't see particles on walls yet as the particles have not got far enough in the flow to hit the walls. The "Waiting for next time step" count shows all these particles are in the flow and still moving along.

I imagined that was the case, thanks for the confirmation.

Originally Posted by ghorrocks

I would recommend you check whether the poorly converged SS run is still good enough (see the FAQ). It probably is still good enough to use and transient is not required, but you should check.

how can i judge if it is good enough? the problem is that as the monitor bounces, the number of particles collected on the walls change too much (from 30% to 90%), which is the only data I need from this.

Originally Posted by ghorrocks

Why are you using a time step size of 10^-4? If you have not set the time step size with a sensitivity analysis then it is almost certainly wrong. I would recommend you use adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size are wide enough you never hit it, and make the initial time step size the 10^-4 you are currently using.

I ran it as adaptive, 3-5 coeff loops. the timestep that gave me a courant < 1 along with residuals between 10^-5 and 10^-7 is 2e-4, so I adopted it as fixed timestep and ran it. 3e-4 already increases courant to 1.20. from what I read, courant should be <1, so this is the reason I chose the given timestep.

[ghorrocks]

I ran it as adaptive, 3-5 coeff loops. the timestep that gave me a courant < 1 along with residuals between 10^-5 and 10^-7 is 2e-4, so I adopted it as fixed timestep and ran it. 3e-4 already increases courant to 1.20. from what I read, courant should be <1, so this is the reason I chose the given timestep.

No, that is not the correct approach. When you run adaptive time steps with 3-5 coeff loops it automatically adjusts the time step size depending on the mesh and physics, but also the convergence criteria you use. So as you tighten the convergence criteria the time step will get smaller, and as you loosen it the time step size will get bigger.

When you are setting up a simulation you need to validate the mesh, convergence tolerance and time step size (if transient) you are using are going to give you the accuracy you need. The sensitivity study you use to confirm this is often difficult and often iterative - you work out an initial mesh, then the convergence tolerance and then the time step size, and then you check the mesh size again and it has moved - so you have to go around the whole cycle again and iterate until all three of them are OK simultaneously.

The advantage of adaptive time stepping is that it removes the need to work out a time step size, it is done automatically for you. Iterating on 2 parameters is MUCH easier than iterating on 3 parameters, so this is a major saving of time and effort.

When you artificially increased the time step size you just resulted in a combination of a slower simulation (as it is doing more coeff loops per iteration) and a looser convergence tolerance. Not optimal.

And I repeat - ignore Courant Number in CFX. It is an implicit solver and has not Courant Number restrictions. Courant Number = 1.0 is a hard stability limit in explicit solvers and that confuses people into thinking it must be important in CFX as well. You should do a sensitivity analysis to set the time step size, or use adaptive time stepping.

So I recommend putting the adaptive time stepping back on, and do a sensitivity study on convergence tolerance to see how tight you need to converge. Do do this, compare the results at a convergence tolerance of 1E-4 and 1E-5. If they are the same then 1E-4 is fine to use. If they have significant differences then try 1E-6 and compare 1E-5 and 1E-6. If they are the same then 1E-5 is OK to use, but if not the keep tightening it until you find it.

[lgtmelo]

Originally Posted by ghorrocks

So I recommend putting the adaptive time stepping back on, and do a sensitivity study on convergence tolerance to see how tight you need to converge. Do do this, compare the results at a convergence tolerance of 1E-4 and 1E-5. If they are the same then 1E-4 is fine to use. If they have significant differences then try 1E-6 and compare 1E-5 and 1E-6. If they are the same then 1E-5 is OK to use, but if not the keep tightening it until you find it.

ok! for this cases do I keep adaptive time step until the end of the run? because last time I did this it eventually got to 1e-10, which is when I gave up and adopted a reasonable fixed timestep from this run.

[lgtmelo]

is this what you mean for this first attempt now?

[ghorrocks]

If the time step size spirals to nothing it is showing that it is having a hard time converging, no matter what you do. You should then think about what can you do to improve the numerical stability and make it easier to converge:

* Double precision numerics
* Improve mesh quality
* Better initial condition
* Improve mesh quality - important enough to say twice

Anything you can do which improves mesh quality will make everything easier. So time invested in a better mesh will pay you back tenfold down the track. Spend a bit of extra time here and make sure it is the best you can do.

[ghorrocks]

Yes, they look like good settings for a convergence tolerance = 1E-4 run.

[lgtmelo]

Originally Posted by ghorrocks

If the time step size spirals to nothing it is showing that it is having a hard time converging, no matter what you do. You should then think about what can you do to improve the numerical stability and make it easier to converge:

* Double precision numerics
* Improve mesh quality
* Better initial condition
* Improve mesh quality - important enough to say twice

Anything you can do which improves mesh quality will make everything easier. So time invested in a better mesh will pay you back tenfold down the track. Spend a bit of extra time here and make sure it is the best you can do.

I actually spent the past week before making this post improving the mesh because I thought this would be what was holding the convergence from happening. I based my changes in a lot of reading from here - and that means there were a lot of changes. in the end I redid the proximity and curvature with higher sizes (0.5mm), that way I made sure there were no drastic changes with the actual mesh from the medium (used 1.5mm size and 2mm max size there). for the inflation I calculated the Y+ and used first layer thickness. 0.4 for skewness target. in the end it seemed very much better than what I had made a month ago... I put the adaptive run to go and will check it tomorrow. hope it gets somewhere, because I dont know what else I could do for the mesh.

and as for double digits precision, its been on since i began.

again, thank you for contributing with your time to my model. i trully appreciate and hope one day to pay it forward.

[lgtmelo]

here is the new ongoing run with adaptive and 1e-4. tomorrow i will let you know how it is

[ghorrocks]

Note that y+ is meaningless in a laminar flow. You need to work out mesh settings in laminar flow with a sensitivity analysis.

[ghorrocks]

There are a few ways you can tell if a transient simulation is required:

1) Run it SS and converge as tight as you can. Then look at the resulting flow field in CFD-Post and see if you can see signs of transient flow - this will probably take a bit of experience to know what to look for. But if you add the equation residuals to the results file (on the output tab) you can then see the regions of high residuals as these are the regions which are holding up the convergence. You have to assess whether the transient flow it is showing is significant for the results you want or not.

2) Run it transient and see if it settles down to SS. Then it is definitely SS, it just needs a transient run to get there. You might be able to get this to converge with a SS run with better settings.

3) Run it transient and look at animations of the flow field to physically see the transient behaviour. While this is the clearest and most definitive way of doing it, it is also the slowest as the run will take a while to complete.

[lgtmelo]

good morning gentlemen! so this is what I got from the transient + adaptive + 1e-4 run:





i am thankful for the instructions i have been getting. as of this run, I understood how the residual limitation is imposed from seeing the graph (as it reaches the 1e-4, it changes the courant - which I now know is not my priority - so it lowers residuals once again).

however, I have some questions regarding the output. the first is regarding this warning that I got. should I ignore it as the number of failures is so low when compared to the iterations or is it meaningful:

================================================== ====================
Convergence Warnings Summary
================================================== ====================

+-------------------------+------------------------------------------+
| Equation Class | Solve Location | Number of |
| | | Convergence |
| | | Failures |
+-------------------------+------------------------------------------+
| Momentum and Mass | DEFAULT | 7 |
+-------------------------+---------------------------+--------------+



second question is about the number of particles that are being deployed. by the last iteration, this is what I got:

+--------------------------------------------------------------------+
| Particle Fate Diagnostics |
+--------------------------------------------------------------------+
| Particle type | Fate type Particles |
+--------------------------------------------------------------------+
| BACTERIA | Entered domain : 29 |
| | Continue from last time step : 4723 |
| | Left domain : 26 |
| | Collected on walls : 8 |
| | Waiting for next time step : 4718 |
+--------------------------------------------------------------------+


can I have this somehow like how steady state is shown (1000 particles entering, X particles collected on walls, Y particles left domain), so I can stablish a ratio of collected particles?


best regards to everyone involved

[lgtmelo]

Originally Posted by ghorrocks

So I recommend putting the adaptive time stepping back on, and do a sensitivity study on convergence tolerance to see how tight you need to converge. Do do this, compare the results at a convergence tolerance of 1E-4 and 1E-5. If they are the same then 1E-4 is fine to use. If they have significant differences then try 1E-6 and compare 1E-5 and 1E-6. If they are the same then 1E-5 is OK to use, but if not the keep tightening it until you find it.

quick question: as i finished the run for 1e-4 tolerance, i changed PRE to 1e-5 and ran again. it took a mere 1 iteration, as it lowered residuals to 1e-5 and finished. should i clear generated data beforehand so it runs the whole iterations again or is this fine?