CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Disturbed flow field at outlet boundary (Multiphase flow through pipe) (http://www.cfd-online.com/Forums/cfx/74385-disturbed-flow-field-outlet-boundary-multiphase-flow-through-pipe.html)

Michiel March 31, 2010 05:01

Disturbed flow field at outlet boundary (Multiphase flow through pipe)
 
2 Attachment(s)
I'm want to analyse the transport of high density sand/water mixture throug a horizontal pipe with a diameter of 105 mm and a length of 3000 mm (3 m). The sand is defined as dispersed solid with a packing limit of 0.63 and a particle size of 0.2 mm. For the drag force i use the pre defined Gidaspow model. Bouyancy is activated.

At the pipe inlet I have a uniform velocity which varies from 0.5 m/s up to 5 m/s. The volume fraction of sand is set to 0.4 and for water to 0.6. Before simulating the actual mixture I run a water only case which provides the initial flow field for the final analysis.

The outlet is defined as average static pressure set to 1 bar. Reference pressure in the domain is also set to 1 bar.

I inserted 2 pictures. On the picture of the outlet you can see the volume fraction of sand expressed in colours.

Attachment 2753

Because of the bouyancy the sand wants to concentrate on the bottom of the pipe. I would expact after 3 meters of pipe length, there should be a stable flow flied. But as you can see, in the region near the outlet there is an inconsistancy. Also the velocity vectors are showing a slightly donwards flow at the outlet boundary. How can this happen?

The second picture is showing the inlet of the pipe.

Attachment 2754

It is clearly seen that the inlet has an uniform mixture. The sand tends to sink slowly as it gets further away from the inlet. After about 1 meter the flow flied reaches a stable situation, which remains there until it comes verry near the outlet.

Why is the flow flied not stable at the outlet region? Did I define the outlet boundary (average static pressure, 1 bar) wrong?

I tried several options, but i cannot get a proper result out of this...

ghorrocks March 31, 2010 07:05

Have you tried using a velocity outlet and a pressure inlet? Just a guess.

Michiel March 31, 2010 07:15

Well, I thought I had. But I was just searching for the files, and i can't find them. It would be quite stupid to forget this option....

I will try this right now, and comment later.

Michiel March 31, 2010 09:28

Just finished the calculation... Results don't look good.

Almost during the complete solution a wall was placed at the inlet, at the last iterations about 45% of the area was blocked. Convergence history looks like shit. Also the volume fraction of sand is I don't think this is the way to go...

Most of the basic settings as I described in the first post came from the following model: http://works.bepress.com/sandip_lahiri/23/ The model I use has been successfully used by the author of this thesis.

Do you have another suggestion?

feizaghaee March 31, 2010 10:30

have you tried a Known pressure feild as outlet BC?
i suggest at frist simulate a pipe without sand and investigate the velocity feild then try multiphase.

ghorrocks March 31, 2010 17:57

Also don't forget to try the pressure averaging options on the outlet BC. They might help.

Michiel April 1, 2010 02:52

2 Attachment(s)
Yesterday I couldn't fix it. Now i'm concentrating on the water only calculation. It seems the problem is not only present for the two phase flow.

I have plotted the pressure contours near the outlet boundary for the water only flow:

Attachment 2765

It is clearly seen that the outlet boundary (right) has an influence on the pressure distribution.

The velocity profile:

Attachment 2766

I would think the flow behaviour at the outlet should be the same as any cross section in the pipe where a fully developed flow field exists, or am I missing something?

ghorrocks April 1, 2010 06:30

As I said in my previous post, have you tried the pressure averaging options? I suspect this may be caused by the average static pressure option you are using.

Michiel April 1, 2010 10:44

Yes, all calculations performed with average static pressure outlet, the pressure averaging option was set to "average over whole outlet". I also tried the other option "circumferential" with the pipe center line difened as axis. This resulted in an error when the calculation reached the convergence target.

Also tried a mass flow rate outlet, but still no improvement.

I think I start all over again:confused:...

ghorrocks April 2, 2010 06:09

Quote:

all calculations performed with average static pressure outlet
That's my point. Have you tried turning pressure averaging off and specifying a pressure over the whole boundary?

Michiel April 2, 2010 08:04

1 Attachment(s)
Ow sorry, I misunderstood you.

I also tried a static pressure outlet without averaging. The velocity profile looks better, but still there is a change near the boundary, see:

Attachment 2787

ghorrocks April 3, 2010 06:29

Are you sure your simulations are adequately converged and the mesh is of adequate quality? The bumpiness in your contour lines could be a sign things are not right there.

Michiel April 7, 2010 02:44

1 Attachment(s)
Solution is converged to target 1e-4. I also think there is something wrong with the mesh.

Mesh at outlet:
Attachment 2846

That is what i meant by starting al over again; building a new mesh.

Michiel April 7, 2010 08:20

1 Attachment(s)
I made a simple extrude mesh with hex elements. The velocity profile looks much better now:

Attachment 2849


There are no inflation layers, this is net yet the final mesh. I have to focus more on my meshing skills to get a proper mesh. So i will have some work for next week.

Thank you for your comments!

ghorrocks April 7, 2010 18:38

Convergence to 1e-4 is generally loose convergence. I suspect your simulation is not fully converged yet. Do a sensitivity check on the convergence tolerance before changing anything else - there is not point working on a partly converged solution.

freemankofi April 8, 2010 16:36

hi Michiel,
1. I think using specifying 1bar pressure at the outlet means you're intrucing more errors into your solution filed. remember, is only pressure gradient is important in your governing equation. Therefore, setting reference pressure to 1bar, allows you to specify Zero at the outlet. In such a case, you reduce your error and therefore getting converged solutions. For a single phase flow (water) this shouldn't be a problem in CFX. If still, then I think you've more 'fundamental' problem than BC.

2. As for solid-liquid flow, is your flow laminar or Turbulent? My experience is that for turbulent you shouldn't be a problem if you run it in 'transient' mode. For laminar, I'm having a big challenge here. I had converged solution, however, my VF is wrong. CFX indicates that there's suspension/transportation of the sand, meanwhile, experiment indicate that there's no suspension of the sand and only a fraction of the sand is delivered.

All the best

Michiel April 21, 2010 04:28

Thank you both for your advice.

I changed the unstructured mesh to a structured O-grid. The first calculations have no difficulty to converge to 1e-5. I will try to set the outlet pressure to 0 en see if this works out positive. Maybe I try a transient analysis. I still have a little difference in concentration profiles at the end of the pipe and just before the end of the pipe.

Eventually i want to use the two phase model for turbulent pump calculations. The current analyses i use to get familiar with two phase cfd and to build a basic model which should be usable in slurry pump simulations.

@freemankofi, I saw you postings about your problem. What you want to model is much more difficult I think. As I mentioned in a reaction on one of your postings, i think the settling of the solids is verry hard to model.

freemankofi April 21, 2010 10:14

Michiel,

I wouldn't use the exact pipe length due to influence from outlet BC. If original pipe length is say, 10m, you want to add couple of meters to it. In such a case you don't extract your results from outlet but around 10m instead. This will avoid any outlet BC effect. If it is a fully-developed flow problem then, try to used normal single phase flow expression to estimate your entry length and here, add reasonable extras length to accommodate the outlet BC.

If you have an idea about the outlet quantities such as volume fraction or concentration, then you might consider using "opening with p_spec=0" at the outlet. This BC is more robust and tend to give better convergence.

Caution should also exercise when you're setting-up your final pump problems, especially the BCs. Here, you want to extend the domain such that any BCs will have no effect on the results.


All times are GMT -4. The time now is 23:04.