CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Backflow at outlet in a Eulerian gas-solid simulation (http://www.cfd-online.com/Forums/cfx/108393-backflow-outlet-eulerian-gas-solid-simulation.html)

audrey October 22, 2012 14:22

Backflow at outlet in a Eulerian gas-solid simulation
 
1 Attachment(s)
Hi everyone,

Does anyone have experience with simulating dense gas-solid flows using a Euler-Euler approach in CFX? I've been working on this problem part-time for almost two years and I still haven't made a breakthrough.

The current problem is that I eventually get gas backflow through my pressure outlet (CFX places a wall at the outlet), no matter the timestep I choose. The backflow is small initially, but increases steadily and doesn't recover.

My geometry is as simple as can be (long tube with inlet at one end face and outlet at the other). My mesh is as fine as our CFX licenses will allow and all mesh statistics are good. I also kept the physics as simple as I could. I kept the solid volume fraction very low to start, because my simulations were giving me overflow errors at higher volume fractions.

When I perform the exact same simulation with only gas, convergence is reached quickly and I have no issues whatsoever.

I must be doing something very silly and obvious, but I've gone through all the suggestions on improving convergence and nothing still.

I'm attaching the CEL from my latest simulation. The level of convergence is very high at the end of each time step (RMS e-7 or lower for all variables), but the problem still occurs. I stopped the simulation even if the backflow problem was small because I experienced the same issue in the same simulation with larger time steps and the percentage of backflow increased steadily after that.

Any help would be immensely appreciated.

Thanks,
Audrey

ghorrocks October 22, 2012 17:45

Can you post an image of your geometry and what the flow looks like when you get back flow? Also an image of what you expect the flow to be would be good.

audrey October 23, 2012 05:19

4 Attachment(s)
I have attached a picture of the geometry. It's a 3m long cylinder, with inlet at one end, outlet at the other and a wall in between. The actual geometry I would like to simulate is a bit more complicated, but I simplified it to start.

I've attached some images of the flow behaviour just before backflow occurs. As expected, the particles are concentrating at the bottom of the cylinder (they should form a bed) and the gas is flowing from inlet to outlet above the bed.

Oh, perhaps I should clarify, only the gas is wanting to backflow through the pressure outlet.

ghorrocks October 23, 2012 18:52

I do not think this geometry simplifies the simulation and that is the cause of the problem. Your end boundary conditions have the particles falling parallel to the BC, and the flow going in and out. This is a complex BC and will always be numerically unstable.

A better BC is one where the flow direction is the same direction across the whole BC, and the flow is close to normal to the BC surface. This is numerically much easier to handle.

audrey October 24, 2012 04:41

1 Attachment(s)
Hi Glenn,

Thanks for the response. I'm not sure I'm following your advice however.

Can you elaborate a little on how I could achieve the kind of boundary condition you are talking about in this specific case?

The way I see it, there are two options for boundary conditions:either a) the back face is an outlet, as in the geometry I showed, or either b) a thin strip of wall at the end of the cylinder becomes the boundary (see sketches attached).

The main flow features should be horizontal: the particles should settle near the inlet and then slowly roll towards the outlet. They will then fall out once they reach the outlet. The gas flow is currently parallel to the walls of the cylinder, but will eventually be heated, so that gas will want to exit upwards.

Should I change the geometry to something like my sketch b, or can you think of a different geometry that would give better boundary conditions?

Thanks for your help,
Audrey

ghorrocks October 24, 2012 05:32

Typically this is done by extending the BC upstream or downstream to where the flow is simpler. In this case I would consider extending the inlet upstream to where it is only gas entering. Then the solid enter from a port in the side I guess.

audrey October 24, 2012 05:50

Are you thinking that the inlet boundary is the problem rather than the outlet? The flow seems to develop as I would expect beyond the inlet.

I'm aware that this is a challenging simulation to achieve, but I'm actually not very interested in the gas flow at the inlet. In the final simulation (if I ever get there) there will be pyrolysis reactions, so the gas flow from the inlet will be replaced with gas evolving from the bed of particles. But before I can make that happen, I need to manage a cold simulation of the flow of solids.

Is there any way I can do a simulation with no gas flow and only solids entering and leaving, or is that a recipe for disaster (as I imagine it would be)?

Or should I actually try to run the simulation with an opening instead of an outlet?

I'd like to better understand why I get backflow at the outlet actually. Given the flowrate of gas entering through the inlet, why would the gas be drawn in through the oultet? Is the flow itself creating a suction on the outlet? Does it have anything to do with the flow of solids? Or is it just a numerical artifact?

Again, thanks for any help you can give. If I can't get this working in the next couple of weeks, I will have to move on to something else.

ghorrocks October 24, 2012 06:00

At the moment I think both the inlet and outlet are problems. But I suspect the outlet will settle down in time, but the inlet needs a fundamental rethink.

I realise you don't care about the flow upstream, but you may need to put it in anyway for numerical stability. The location of BCs is determined on where you can specify BCs properly, not by your region of interest (but obviously the BCs need to enclose your region of interest).

You can always turn bits of the simulation on and off with expert parameters, or use a single phase model as an intial condition.

Yes, using an inlet at the inlet and an outlet at the outlet may help. You will get lots of warnings about reverse flow until it settles down but if it works then go for it.

You will have to look at your simulation in detail to work out where the back flow is coming from. It could be from the solids, it could be numerical noise.

audrey October 24, 2012 07:07

Thanks for your suggestions.

Can you clarify what you meant by "using an inlet at the inlet and an outlet at the outlet"? I'm lost - did you mean using an inlet at the oulet and an outlet at the inlet?

One thing that I'm unclear about is whether I can have a volume fraction of 1.0 for the dispersed solid phase. What I'm thinking is that I could physically separate the gas and solid boundary conditions, at least until I get convergence. But will the solver trip over 100% dispersed solids?

singer1812 October 24, 2012 09:21

That is where Glenn was heading with his post. Separate the solid and gas inlet BCs.

ghorrocks October 25, 2012 06:15

By "using an inlet at the inlet and an outlet at the outlet" I mean use inlets and outlets, not openings. Openings allow backflow and that can be numerically difficult. Inlets and outlets do not allow backflow and that may improve stability enough that it runs.

As Edmund says, an even simpler approach is to have a main inlet further upstream where only pure air comes in to establish the air flow, a port at the side with solids and air to inject the solids. This approach means the air flow is established when it gets the solids and the inlet never sees backflow, especially backflow with solids.


All times are GMT -4. The time now is 02:01.