[lgtmelo]

hey, just finished the 1e-5 run! here are the pics:





cant tell if it is fine or not. also got the same errors but in greater amount (assuming it is because resolution increased):

| Equation Class | Solve Location | Number of |
| | | Convergence |
| | | Failures |
+-------------------------+------------------------------------------+
| Momentum and Mass | DEFAULT | 22 |
+-------------------------+---------------------------+--------------+


and the particles:

+--------------------------------------------------------------------+
| Particle Fate Diagnostics |
+--------------------------------------------------------------------+
| Particle type | Fate type Particles |
+--------------------------------------------------------------------+
| BACTERIA | Entered domain : 5 |
| | Continue from last time step : 5745 |
| | Left domain : 1 |
| | Collected on walls : 2 |
| | Waiting for next time step : 5747 |
+--------------------------------------------------------------------+

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


gonna stand by now and wait for any opinion from Glenn

best regards!

[ghorrocks]

These results are suggesting it definitely is transient, and quite strongly so. You should have a look at the post processor for the last third of the run to see if you can spot where the transient behaviour is occurring. It appears to be quite strong, based on the velocity monitor point results so it should be easy to spot.

You then need to decide whether the transient feature is important enough to need to be included for the results you want to get. If you post an image of what you think is the transient bit that would be good.

As I said previously, you are not getting particles hitting the wall or exiting the domain (like you do in SS runs) as in transient runs the particles advance through the domain one time step at a time, and they have not been simulated long enough to hit a wall or exit yet. They are all in the middle of the flow, still moving along. You do not get this SS as the particle tracks are assumed to happen instantaneously, so all particles are just integrated out to their end fate - no particles are still in the flow.

[lgtmelo]

Originally Posted by ghorrocks

These results are suggesting it definitely is transient, and quite strongly so. You should have a look at the post processor for the last third of the run to see if you can spot where the transient behaviour is occurring. It appears to be quite strong, based on the velocity monitor point results so it should be easy to spot.

hey Glenn, thanks for the answer! what exactly am I looking for here when I load the results in the post? should I use the 1e-4 or -5 run?

thanks!

[ghorrocks]

Use either.

But compare the 1E-4 run to the 1E-5 run to see if you can see significant differences. It is probably too early to be sure in your case as the significant thing in your case is how much bacteria ends up on the walls (from what I understand of your work).

[lgtmelo]

how do I spot where the transient behaviour is occurring?

[ghorrocks]

Have you had a look? It might be obvious. If not post some images here and we can help.

Also, generating some transient animations of the flow might help as well (only for the last third of the time steps, you don't care about the startup transient).

[lgtmelo]

Originally Posted by ghorrocks

Have you had a look? It might be obvious. If not post some images here and we can help.

Also, generating some transient animations of the flow might help as well (only for the last third of the time steps, you don't care about the startup transient).

not yet! getting home in 10 and will do! thanks

[lgtmelo]

pics for 25 particles:

[lgtmelo]

from POST i can see a slight deviation of the particle path when it is about to enter the infill, and a big deviation right after it leaves.

[lgtmelo]

i'm trying to do a count of how many particles cross a plane so i'd know how many stood behind in the infill. any ideas? I created a plane by the exit, but cant find a variable that would tell me so.

[lgtmelo]

hey, so i was able to do one thing:
I created two particle track display for my domain, and could filter particles according to were they END. so it shows 1014 particles going up to OUTLET, and 1795 going up to INFILL. that would be exactly what I need, BUT there is the fact that some particles, by the current ending step on solver, were still on displacement (like on their way somewhere), and then when the iterations stopped, they ended like in the middle of nowhere. i.e., I have 7526 tracks, 1014 finishing on OUTLET and 1795 finishing on infill. if I keep iterations running, I will always have new particles being injected as per the mass flow of 0.12kg/s. and not all of the particles will reach INFILL or OUTLET, simply because they didnt have time to.

is there any way to exclude these from my results so I can analyze a specific amount that had time to cross all my domain and see which stuck on INFILL and which went through to OUTLET?

pic below shows how that 7526 - (1014 + 1795) particles didnt have time to reach any boundary. but they might have, if they had time. so I can't affirm 1795 out of 2809 (63.9%) is my adhesion rate, because particles reach INFILL in less time than it takes particles that went through it to reach OUTLET...

im having a hard time expressing myself, did it make sense to anyone?

[ghorrocks]

There is quite a lot there....

Firstly, I would not look for transient flow in the particle tracks. It is more likely to be in the velocity or pressure field. So do a plane through the middle and colour it by velocity or pressure. This will show the transient features more clearly.

But I see the tracks coming out of the infill have lots of weird kinks and wobbles in them. Some even loop around and go back into the infill. This is highly likely to be significantly transient I suspect, but look closely to confirm (as if this is transient it is MUCH harder and slower to solve. You only want to go transient if you really have to).

I note your averaged volume fraction goes up to around 377. Volume fraction should not exceed 1.0, and the Lagrangian particle tracking model is only valid in much lower VF than that (upper limit of 0.1 to 0.3). Check your particle definition because something is very wrong here.

Don't worry about interpreting the results yet. There are still basic questions (eg: is it transient) and fundamental errors to fix (eg: volume fraction of particles = 377) first.

[lgtmelo]

hey Glenn, good morning!

here are pics of a middle plane with contours of pressure and velocity.

ps: just learned how to upload pics as thumbs so forgive me for all the previous visual polution.

best regards!


glenn.jpg
glenn2.jpg

[ghorrocks]

Those images do not show much. You will have to zoom in much closer to the infill section.

[lgtmelo]

Originally Posted by ghorrocks

Those images do not show much. You will have to zoom in much closer to the infill section.

Hi Glenn!

Here are new pics

Best regards!

glenn.jpg

glenn2.jpg

[ghorrocks]

I cannot say anything definite about that. You will have to do some animations of it.

The mesh artefacts suggest you are still running quite a coarse mesh. Have you done a mesh refinement study yet? In my work looking at particles hitting walls you need very fine meshes to get these effects accurate.

[lgtmelo]

Originally Posted by ghorrocks

I cannot say anything definite about that. You will have to do some animations of it.

The mesh artefacts suggest you are still running quite a coarse mesh. Have you done a mesh refinement study yet? In my work looking at particles hitting walls you need very fine meshes to get these effects accurate.

just let me know what animations you need and ill generate them

in my poor experience, the mesh is quite ok. but again, look how many mistakes i have made so far how can I test it?

ill board a flight now, but just post what u want me to do and ill answer in 12h. thank you!

best

[ghorrocks]

Do a transient animation of that plane for velocity and/or pressure to see if it is transient.

The parameters you need to check you have set accurately are mesh size, convergence tolerance and time step size (if transient). Some simulations also need to check boundary proximity, and some physics models also have tuneable constant (eg particle tracking has a few). You need to show that you have set these parameters to give you the accuracy you require.

The simplest way to do this is with a sensitivity analysis. Taking mesh size for an example: run the simulation with a given mesh, then run it again with a mesh with half the edge length (so around 8 times the element count in 3D). Compare the two simulations, and if the results on parameters you care about are the same within a tolerance you are happy to accept then the coarser mesh is OK to use. If not, then refine the mesh by a factor of 2 again and repeat. Keep going until you have found the mesh size which gives the accuracy you require.

[lgtmelo]

hi glenn, sorry for taking so long.

is this what you wanted: nevermind, noticed it isn't. will post the correct animation soon!

thanks

[lgtmelo]

Pressure: https://i.imgur.com/A3ymcGt.mp4

Velocity: https://i.imgur.com/nFmDbZO.mp4