[ArtSimulatingLife]

Hello, I have geometry which consists of a small inlet pipe which turns 90deg, expands into a rectangular cross section, turns back through 90deg and back to a small pipe at the outlet. I'm using Lagrangian one way coupled particle tracking, when the particles exit the inlet pipe a large proportion of the particles are thrown against the walls and get trapped despite the coefficient of restitution being 1. This does not happen experimentally. I feel as though the problem comes due to the particles being point masses, meaning they get closer to the wall than is physically possible and thus stuck in the boundary layer although I'm not sure. At the minute less than 10% of my particles leave the domain, increasing the number of integration steps and increasing the total tracking time doesn't help the number leaving the domain.

Does anyone have any advice on how to prevent the particles getting stuck on the walls? Thanks a lot.

[ghorrocks]

The first thing to look at is the particle fate table in your output file. This says where all the particles are ending up. Once you know where they are ending up you can then decide if that is appropriate or not.

[ArtSimulatingLife]

Originally Posted by ghorrocks

The first thing to look at is the particle fate table in your output file. This says where all the particles are ending up. Once you know where they are ending up you can then decide if that is appropriate or not.

I know where they're ending up, they're exceeding the time and the integration limit as they're getting stuck to the wall, increasing both settings does nothing to increase the number of particles leaving the domain.

[ghorrocks]

Is the flow turbulent? If so, have you activated turbulent dispersion?

[ArtSimulatingLife]

Originally Posted by ghorrocks

Is the flow turbulent? If so, have you activated turbulent dispersion?

Yes the flow is turbulent and I have the turbulent dispersion force on.

[Gert-Jan]

Don't let us guess: show the geometry with the particle tracks.

[ArtSimulatingLife]

Originally Posted by Gert-Jan

Don't let us guess: show the geometry with the particle tracks.

I can't show you it unfortunately, I'll try and mock something up later to show you. I'm thinking it's the size of the particle being too large for the cell size that is the issue as with smaller particles the majority make it through. You don't know a way to stop the particles getting closer to the wall than is possible do you?

My thought was run the flow simulation, create a new mesh which is the radius of the particle smaller all the way around, interpolate the results field onto the new smaller mesh leaving behind the region the particles wouldn't be able to physically enter and then run the particles through it. Not sure if this will work or if there's a neater way to deal with large particles on a relatively fine mesh?

[Gert-Jan]

In my simulations I also have particles that get trapped. Especially in certain recirculations on surfaces Not much you can do about it.

However, I noticed you run one-way coupling. Might be better to use two-way coupling. Turning gravity on might also help. But I assume you have that.
Other things to check are drag coefficient, relaxation coefficients, etc.

[ArtSimulatingLife]

Originally Posted by Gert-Jan

In my simulations I also have particles that get trapped. Especially in certain recirculations on surfaces Not much you can do about it.

However, I noticed you run one-way coupling. Might be better to use two-way coupling. Turning gravity on might also help. But I assume you have that.
Other things to check are drag coefficient, relaxation coefficients, etc.

Yeah I have gravity on, I'd rather not have to use two way coupling (wouldn't we all) but I'll give it a try and see if it helps. I wouldn't mind a few particles getting stuck, when I was running smaller diameter populations of particles I was getting about 5% of the particles trapped which is fair enough, now though I'm getting 90% failing to leave the domain and know from experimental results that this isn't physical at the mass flow rate I'm running which is confusing. The drag coefficient and the relaxation coefficients I have no experience with, I'm using the Schiller Naumann model so I believe I shouldn't have to touch the drag coefficient and I don't really know what the relaxation coefficients are.

Edit: in case it's relevant gravity makes things worse but I need to model it, which points towards the mass flow rate not being high enough or the density being incorrect but I've triple checked it all and can't see a mistake

[Gert-Jan]

reduce the relaxation parameters in Pre.

solver settings > particle control > somewhere

[ghorrocks]

My comment here is that if the simulation is showing large particles are getting stuck in the boundary layer but that is not physically realistic then you need to add the physics which push the particles out of the boundary layer, not introduce some artificial and non-physical effect to push them out.

For instance if you look at the Eularian particle tracking model there are several wall lubrication force models. Is an effect like this occurring? These effects are not modelled in the Lagrangian model, so if this type of effect is important you would either need to move to a Eularian particle model or add the physics to the Lagrangian model yourself.

[ArtSimulatingLife]

Originally Posted by ghorrocks

My comment here is that if the simulation is showing large particles are getting stuck in the boundary layer but that is not physically realistic then you need to add the physics which push the particles out of the boundary layer, not introduce some artificial and non-physical effect to push them out.

For instance if you look at the Eularian particle tracking model there are several wall lubrication force models. Is an effect like this occurring? These effects are not modelled in the Lagrangian model, so if this type of effect is important you would either need to move to a Eularian particle model or add the physics to the Lagrangian model yourself.

Unfortunately I can't move to an Eulerian method as I need to get the discretised track information present in the .trk file out to use in something else. What does adding physics to the Lagrangian model entail? Does it have to be done via user Fortran and do you know of any similar tutorials? Someone suggested to me that the issue may be arising due to the lack of a lift force in the Lagrangian tracking model which would naturally push the particles away from the wall due to difference in pressure on either side.

[ghorrocks]

Unfortunately I can't move to an Eulerian method as I need to get the discretised track information present in the .trk file out to use in something else.

You can create particle tracks from a Eularian particle model by post-processing stream lines using the particle phase in CFD-Post.

Adding physics to the Lagrangian model means writing your own particle force function. There are examples of this in the CFX documentation. If you are going to write a function to do a lift force near the walls, you will have to think about what the physics is on a particle level and write a function to describe that. If this was easy it would already be in there. But note the Eularian particle model already has functions to do this

[ArtSimulatingLife]

Originally Posted by ghorrocks

You can create particle tracks from a Eularian particle model by post-processing stream lines using the particle phase in CFD-Post.

Adding physics to the Lagrangian model means writing your own particle force function. There are examples of this in the CFX documentation. If you are going to write a function to do a lift force near the walls, you will have to think about what the physics is on a particle level and write a function to describe that. If this was easy it would already be in there. But note the Eularian particle model already has functions to do this

In the solver modelling guide? I thought I looked in there and couldn't see anything, I'll have another look tomorrow, thanks.

[Gert-Jan]

I would go the CFX-Pre, define a new material as Particle Transport Solid. Then in the Fluid Pairs Tabs, you will find the drag and non-drag forces. Press F1 for the help on what is available.

Look at paragraph: 8.5.4.2.1. Particle User Source Example
Also, look ar paragraph 7.8.2 on Lift Force. It says:

The lift force is proportional to the continuous phase density. Hence, it is mainly significant when the dispersed phase density is either less than, or of the same order of magnitude as the continuous phase density. Also, it is proportional to the continuous phase shear rate. Hence, it is most significant in shear layers whose width is comparable to the dispersed phase mean diameter.
For example, the lift force is important for bubbly flow in a vertical pipe, when the pipe diameter is comparable to the bubble diameter. In this case, the lift force induced by the continuous phase boundary layer is responsible for pushing the bubbles towards the wall. On the other hand, for bubbly downflow, the lift force tends to push bubbles towards the pipe center, leading to the phenomenon of void coring.

I could be totally wrong but if you have heavy particles, this could be a limited contribution. It depends on your continuous phase. If gas, I think lift force will be small. Liquid, it might be necessary.

Also, as you mentioned, Lagrangian particles are point sources without any volume. I have seen examples where in the simulation, the Lagrangian particles got trapped in a recirculation, while in reality a pile of particles ended up, blocking the duct.

Main question is: what is the goal of your simulation?

if your CFD-goal is to prevent the pile from happening, then you might get away with LPT .Then change your geometry to make sure that those reirculation do not occur. If your goal is to match experiments, then you need to finetune particle-particle and particle-wall interaction and make sure the particles have a volume. Then go to Eulerian in CFX or switch to Fluent/Star-CCM+ to use DPM things like EDEM.