[lgtmelo]

Good morning everyone. First of all, thanks in advance to whoever helps me.

I've been struggling with a model for a while now. To be objective, I'm trying to get the collision rate of 1micron diameter solid particles into a filter geometry on a simple tube. SST turbulence, turbulent dispersion force, fully coupled.

To do so, I have set the filter as a Wall with restitution coefficients of 0. From the inlet, 1000 particles run with zero slip velocity. When I run it as steady state, I get the number of captured particles on wall and that's it. However, my simulation never gave me a decent convergence (monitor wouldn't stabilize, residuals wouldn't go below 10^-3). So I studied a lot and improved it using many tips from this forum (thanks for that).

I gave up running as steady state and after running it as transient, adaptive, 3-5 coef. loops, I got the timestep of 1.5e-6; courant of 0 and max courant of 0.06; residuals below 10^-6; flat monitor graph. Ran again as transient using this timestep and everything is beautiful. (steady state reached, I believe?)

But when I run it as transient, I can't get the output I have been working with on steady state: "Entered domain: 1000; Captured on walls: xxxx; Left domain: xxxx". First of all, I only get 1 particle per iteration entering the domain. Secondly, if I understood correctly, for the 8s residence time I have in this model, for 1.5e-6 timestep, I'd need to run the transient model for 5 millions accumulated timesteps for it to end? Or should I just get the 1.5e-6 timestep and put it into the steady state model? Because when I do that, I dont get the same graphs - my residuals won't go as low, and my monitor won't stabilize.

I apologize if that's too big a post, but I tried to give all the info that would help understand my situation.

Best regards!

[ghorrocks]

Thanks for the detailed post. It is very useful when people post what they are doing and other details as then we can understand what you are trying to achieve.

Some comments:
Steady state versus transient - It is quite likely that the flow through this assembly is transient as you will get the flow moving about behind the bluff filter particles. So I would expect that a transient simulation is required. But I would not expect a transient simulation to settle down into a steady state solution. Are you sure you have run the transient solution long enough to see what happens?

Slow particle rate: This is set by the mass flow rate of particles and particle diameter. There are also some particle modelling parameters which affect it as well. So you can increase the number of particles by adjusting these parameters.

Fully coupled versus One way coupling: Are you sure you need this to be fully coupled? If you can run it with one way coupling it will be MUCH easier and a hundred times less CPU time.

[lgtmelo]

thank you for answering Glenn. in my learning curve here, I think your posts from 10+ years ago were already very helpful.

Originally Posted by ghorrocks

Are you sure you have run the transient solution long enough to see what happens?

i am definitely not sure. like i mentioned, if i am correct, id need it to run for 5billion+ timesteps - that is: ~8s time from inlet to outlet (from length divided by velocity) divided by 1.5e-6 (which is the timestep i am using, found from the transient adaptive using 3-5 coef.). is this correct? if so, i'll never run it long enough pic of where it is currently:

Originally Posted by ghorrocks

Slow particle rate: This is set by the mass flow rate of particles and particle diameter. There are also some particle modelling parameters which affect it as well. So you can increase the number of particles by adjusting these parameters.

how I did when in steady state: 1000 particles, 0.12kg/s, 0.065m/s (same velocity of the water medium), all injected with equally spacing from the inlet (left plane in the above pic). that gave me the 1000 divided into collected on walls/left domain. but in transient state, i dont have the field to input the number of particles anymore. it becomes number per seconds. so I do input 1000 [s^-1] and keep the rest just like before (uniform injection, equally spaced, 0.12kg/s; 0.065m/s)

Originally Posted by ghorrocks

Fully coupled versus One way coupling: Are you sure you need this to be fully coupled? If you can run it with one way coupling it will be MUCH easier and a hundred times less CPU time.

i am definitely NOT sure I need to be fully coupled. I just read that it is a more reliable model, since each fluid will "act" into the other, instead of just behaving as if they were independent.

[ghorrocks]

thank you for answering Glenn. in my learning curve here, I think your posts from 10+ years ago were already very helpful.

Glad to be of service! I think my first posts on the forum are actually from 1998 (24 years ago) so my challenge to you is to see if you can find them

Your chart shows it decaying to a flat line. But it is just velocity at a point. The transient stuff is likely to be just behind a bit of your filter. Right in the middle of the filter actually. So you are probably not looking at a transient bit.

Hold off on the transient particles per second for now, I am not convinced you need transient yet.

Yes, fully coupled is a more "reliable" model in that it includes more physics. But the price of reliability is a slower simulation, and in my experience transient particle tracking models can be 100 times slower to run than one way coupled. This obviously depends on exactly what you are modelling, but the point is fully coupled simulations are MUCH slower.

So only use fully coupled if you really need it. In your case, I understand you have 1um particles (meaning they are really small), they appear to be bacteria (meaning the density of them is likely to be about the same as the water fluid) and I do not see anything which generates a big slip velocity between the bacteria and fluid - this all suggests a one way coupled model will be fine.

[lgtmelo]

Originally Posted by ghorrocks

So only use fully coupled if you really need it. In your case, I understand you have 1um particles (meaning they are really small), they appear to be bacteria (meaning the density of them is likely to be about the same as the water fluid) and I do not see anything which generates a big slip velocity between the bacteria and fluid - this all suggests a one way coupled model will be fine.

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).

thanks!


ps: i think the oldest post from you i was able to find was from around 2005 haha. and YES, all of them were very helpful to me.

[ghorrocks]

Transient or steady state is another issue entirely. I would:
* Have a look at your transient final results and see if you can spot where it is transient.
* Run it steady state and include the equation residuals in the results file. Then you can look in the post-processor and see where the high residuals are and this is the problem area.

This will help decide if it is transient or steady state.

Also, I would just run it SS and see if it is different. If no difference then SS should be fine.

Finally - note that turbulent dispersion on particle tracking with coupled particle tracking means a steady state result cannot exist (look this up in the doco). So your lack of convergence might be just the turbulent dispersion model. If this is the case then this will be fixed by going to one way coupled particles (if this assumption is valid).

[lgtmelo]

Originally Posted by ghorrocks

Finally - note that turbulent dispersion on particle tracking with coupled particle tracking means a steady state result cannot exist (look this up in the doco). So your lack of convergence might be just the turbulent dispersion model. If this is the case then this will be fixed by going to one way coupled particles (if this assumption is valid).

that i didnt know! thank you. does this mean that after selecting one-way i have to set turbulent dispersion force to none instead of "particle dispersion"?

[ghorrocks]

You can still have turbulent dispersion in a one way coupled model. It is just that the random jiggling of the particles then does not affect the flow field, so the flow will converge fine.

Also consider whether you actually have turbulent dispersion occurring. The flow in many filters is laminar, so adding turbulent dispersion is not appropriate.

Finally - be aware that the particle tracking model does not have complete physics of whether particles impact the surface or not. For instance the particles are modelled as points and it is assumed they hit the walls when that point passes through a wall. But the actual particle has a diameter, so will hit the wall before its centroid point does. This is not taken into account. There are other more subtle effects not taken into account as well.

[lgtmelo]

disregard the next sentence: thats weird, now solver wont show the "particles source change rate" graph, or mention particles entering/exiting domain or captured on walls. is this because of the one way coupling or did I mess something up?


"One-way coupled particles are solved at the end of the simulation" got it!

[lgtmelo]

Originally Posted by lgtmelo

thats weird, now solver wont show the "particles source change rate" graph, or mention particles entering/exiting domain or captured on walls. is this because of the one way coupling or did I mess something up?

disregard the next sentence: yep, just noticed on pre I cant chose the iteration number to "inject" the particle. can you help me finding out how the number of particles that have collided into my filter now?

"One-way coupled particles are solved at the end of the simulation" got it!

[ghorrocks]

One way coupling does not need to converge the flow and particle coupling (which is what particle source change rate is). It just iterates the fluids then solves the particles once only. No convergence required.

It will show the particles entering/exiting the domain, just in a different part of the output file. Look in the end section.

[lgtmelo]

Originally Posted by ghorrocks

You can still have turbulent dispersion in a one way coupled model. It is just that the random jiggling of the particles then does not affect the flow field, so the flow will converge fine.

Also consider whether you actually have turbulent dispersion occurring. The flow in many filters is laminar, so adding turbulent dispersion is not appropriate.

Finally - be aware that the particle tracking model does not have complete physics of whether particles impact the surface or not. For instance the particles are modelled as points and it is assumed they hit the walls when that point passes through a wall. But the actual particle has a diameter, so will hit the wall before its centroid point does. This is not taken into account. There are other more subtle effects not taken into account as well.

while the model runs: I was originally working with K-E. do you know of any limitation regarding the particle size from it? went to SST because it seems to have the best of both world, but now I am unsure if it was actually an improvement.

thanks

[ghorrocks]

Turbulence model and particle tracking are totally different things. You choose a turbulent model which accurately models the flow, and then the particles do their thing in the flow. There is no direct interaction between the turbulence model and the particles (except when you activate the turbulent dispersion model, and even then the interaction is very diffuse).

I repeat my previous comment: Are you sure this flow is turbulent? Most filters are laminar.

[lgtmelo]

Originally Posted by ghorrocks

Turbulence model and particle tracking are totally different things. You choose a turbulent model which accurately models the flow, and then the particles do their thing in the flow. There is no direct interaction between the turbulence model and the particles (except when you activate the turbulent dispersion model, and even then the interaction is very diffuse).

got it.

Originally Posted by ghorrocks

I repeat my previous comment: Are you sure this flow is turbulent? Most filters are laminar.

I ran it as laminar initially, but solver suggested it was turbulent. also the reynolds it pointed was >5k.

[ghorrocks]

The solver message about turbulence model and Reynolds Numbers are guides only. You should calculate the Reynolds number of the flow yourself - in your case it looks like a tube, so the Reynolds Number from the tube diameter and liquid properties and velocity. Then compare this to known data (eg the Moody Diagram) to work out whether it is laminar or turbulent. And then you select laminar or turbulent based on that.

[lgtmelo]

Originally Posted by ghorrocks

The solver message about turbulence model and Reynolds Numbers are guides only. You should calculate the Reynolds number of the flow yourself - in your case it looks like a tube, so the Reynolds Number from the tube diameter and liquid properties and velocity. Then compare this to known data (eg the Moody Diagram) to work out whether it is laminar or turbulent. And then you select laminar or turbulent based on that.

from the tube only, it would be a laminar flow. but i didn't know if when I add the geometry it would turn to turbulent? the infill has ~3mm diameter passages.

pic of the infill:

[ghorrocks]

Then do a quick calc to see if the filter flow is turbulent: You say the diameter is ~3mm, and look at your simulations to see a typical velocity in them (or estimate the velocity if you can). Then you can get a representative Reynolds Number for the flow in the filter.

(But I know the answer already from experience: If the main flow is laminar then the flow in this infill is going to be laminar as well. This means you can turn off the turbulence model and just model it as laminar, and the turbulent dispersion force option is not available. This will greatly simplify your model.)

[lgtmelo]

Originally Posted by ghorrocks

(But I know the answer already from experience: If the main flow is laminar then the flow in this infill is going to be laminar as well. This means you can turn off the turbulence model and just model it as laminar, and the turbulent dispersion force option is not available. This will greatly simplify your model.)

will do it right now! thank you so much. you have no idea how happy i am haha

[lgtmelo]

quick update while its still running: so far it seems weird. i am considering trying a higher timestep (~7.5s = residence time) . currently on auto, it is 7.76235E-02.

pics:

[ghorrocks]

The turbulence model puts extra dissipation in the model which stabilises it. The k-e model will have lots of additional dissipation, the SST model not so much, but still some. When you remove that dissipation the simulation is more accurate, but more likely to go transient. But this transient flow is likely to be real.

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