# Using RSM model to simulate swirl flow in pipe

• 62 Views
• Last Post 52 minutes ago
KgpNiko16 posted this 18 February 2020

I am trying to simulate the highly swirl flow in confined tube using axi-symmetric swirl (2D geometry).

Version : 2019 R3,R2,R1 (all gives same)

Geometry : 150mm (dia)X 6145 mm(length) rectangle (axisymmetric cylinder)

Working fluid : Air

Model :  RSM , stress-omega

solver : Pressure based

scheme : SIMPLE for coupling , PRESTO for pressure , SOU's for other

Reynolds no : 50 K

Inlet : Velocity profile (axial,radial, swirl)

outlet : Pressure outlet ( Avg pressure = 0)

I am unable to get zero velocity at the axis when RSM is employed but this kind of problem is not there with other turbulence models. Please help.

kkanade posted this 18 February 2020

please cross check with "Modeling Axisymmetric Flows with Swirl or Rotation" in help document. It describes procedure for setting up axisymmetric problems.

KgpNiko16 posted this 18 February 2020

Actually i have followed the documentation rigorously and even tried the step increase of swirl but there is always some finite velocity. Also mesh is sufficiently refined too , though as i refined the mesh the velocity comes down by some amount but to what degree i need to refined is not clear. I mean other turbulence model adhere to the axis boundary condition even at small meshes.

Is there any other way out to solve this issue other than keep on refining the mesh ?

KgpNiko16 posted this 4 weeks ago

Mesh refining is not solving problem, can you tell me about any other possibility ?

abenhadj posted this 4 weeks ago

What should happen at the axis,?

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

Swirl velocity should go to zero. But across one cell width near axis it shows the jump of swirl velocity of order of inlet velocities which is physically not possible.

abenhadj posted this 3 weeks ago

Does it happen with other variants of pressure term? Does it happen with Omega RSM? Does it happen with 3D?

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

3D i have tried but due to big geometry it took me 1 week for 88K iterations till that time there was finite velocity near axis but jump was very less as compared to 2d .

Yes it happen with omega RSM, linear pressure strain and quadratic pressure strain all does the same.

abenhadj posted this 3 weeks ago

How are you quantifying the results? Plots? Via UDF?

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

I am quantifying using CFD post and fluent itself .Also  I am using export data also and even contour plot also.  All give same results..!

abenhadj posted this 3 weeks ago

Can you show the plot out of Fluent? Screenshot of Plot Function + the Plot itself of the swirl component for 2D and 3D.

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

2d simulation results

Non dimensional swirl velocity at different axis stations   ( reference velocity is Uavg based on flow rate)

x099 --> 0.99 m

x1995 --> 1.995 m

x3 --> 3m

x4005 --> 4.005 m

x4995 --> 4.995 m

out --> 6.145 m

x6 --> 6m

x61 --> 6.1 m

Plot function  =   Velocity w / Uavg

3d results are not available at moment , i will add as fast as possible

abenhadj posted this 3 weeks ago

So at the beginning the swirl velocity is zero than it starts deviating right? How does the plot look in Fluent in CFD-Post? How does your mesh look alike? Please increase mesh check verbosity and check values for aspect ratio and cell volume change.

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

What do you mean by beginning ?  Swirl is zero near axis @ exit not inlet. Actually based on my experiments with fluent , Simulation with very high swirl velocity shows high velocity jump near axis but very low swirl velocity it is actually low.  Relative jump probably will be same but i will check that.

This plot is obtained from CFD post which i have taken from presentation which i prepared, that's why black bordered.

Mesh i have already been refining , solution also shows convergence is achieved to the order 1e-5.

That's where is the real problem is, solution shows convergence(residual stagnates) and still we have appreciable velocity jump.

Aspect ratio : it was below 10

cell volume : i didn't checked but i think i didn't gave any high bias factor which might give high volume change .

Mesh : 480 X 1200, near axis cell height is ~1.5e-4 m

abenhadj posted this 3 weeks ago

Cell volume Change was the metric was asking and not the cell volume itself. In order to summarize here:

1/You see a finite value of siwrl velocity at axis which is not physical. This appears with RSM and not with two-equation models

2/You see that 2D and 3D

Is this correct?

What is the boundary condition you provide at your inlet in 2D/3D?

Best regards, Amine

KgpNiko16 posted this 3 weeks ago

Yes cell volume change is metric to quantify the volume change across cells , since my geometry is rectangular so only high growth factor / bias factor can create the large volume change, that i meant.

Point 1 correct ,

Yes 2d case show swirl velocity at axis and 3d case was taking large time so i can't directly conclude that 3d also shows jump but at the time of 88K iteration it had jump in swirl velocity near axis.

Velocity inlet with 3 velocity components profile using UDF.

outlet is pressure outlet with average pressure specification zero

abenhadj posted this 3 weeks ago

RSM models require the best possible mesh quality. High apsect ratio are critical the same with aggressive expansion rates. For that reason Please share information about your mesh quality (increase the verbosity here to 2) and a picture highlighting the mesh.

Best regards, Amine

• Liked by
rwoolhou posted this 3 weeks ago

Are you running double precision, and check [Domain Scale] what the minimum y value is.  Swirl is a function of the tangential velocity and radial position: at the axis these both tend to zero so you need to be careful with mesh [as Amine states] and numerical precision.

• Liked by
KgpNiko16 posted this 3 weeks ago

Yeah i have used double precision and checked the scale too. It shows correct values, min y value is 0.

Actually i am interested in swirl velocity which is equivalent to velocity w,  not related to r=0 anomaly, if i am correct.

KgpNiko16 posted this 3 weeks ago

OKay , i understand, i am listing the details which you have asked.

Mesh Quality:

Minimum Orthogonal Quality = 1.00000e+00 cell -1 on zone -1 (ID: 0 on partition: 0) at location ( 0.00000e+00 0.00000e+00)

(To improve Orthogonal quality , use "Inverse Orthogonal Quality" in Fluent Meshing,

where Inverse Orthogonal Quality = 1 - Orthogonal Quality)

Maximum Cell Squish Index = 0.00000e+00 cell -1 on zone -1 (ID: 0 on partition: 0) at location ( 0.00000e+00 0.00000e+00)

(Cell Squish ranges from 0 to 1, where values close to 1 correspond to low quality.)

Maximum Aspect Ratio = 8.64600e+00 cell 106235 on zone 2 (ID: 106236 on partition: 0) at location ( 4.84796e+00 7.48890e-02)

Minimum Expansion Ratio = 9.91096e-01 cell 445534 on zone 2 (ID: 445535 on partition: 0) at location ( 7.02367e-01 7.46661e-02)

For axis : first cell is 1e-3

For wall : first cell 2e-4

Mesh : 156 X 3224

elements : 502944

KgpNiko16 posted this 2 days ago

Anybody ?

rwoolhou posted this 2 days ago

Sorry, we must have missed this one.

The mesh looks OK. w tends to be the z-component of velocity so isn't necessarily the same thing. Have a look at the contours of angular velocity and post those.

KgpNiko16 posted this 23 hours ago

Here are the contours

1. Inlet region

2. Mid region toward inlet

3. Mid region towards outlet

4. Outlet region

abenhadj posted this 19 hours ago

Add the plot of the swirl velocity along the axis. It should be ideally zero but Fluent uses here cell values. Did you think about refining the mesh towards the axis?

Best regards, Amine

KgpNiko16 posted this 6 hours ago

Here is the plot  : Swirl velocity along axis

I told right , i kept of refining mesh but it was not clear at what point i need to stop. Also already mesh is at 502 K , for student version we have only 512K .

I refined mesh such that in axial direction mesh is reduced and in radial direction it is increased. There was still small jump.

Maximum i went to 480 elements in radial direction.But aspect  ratio went to 65+.

abenhadj posted this 4 hours ago

Let me check again and I will get to you asap.

Best regards, Amine

• Liked by
abenhadj posted this 4 hours ago

Thanks for the patience and also answering our questions all the time. The issue you are observing is a "real" issue and we believe something is missing in our 2d RSM formulation. For that reason we recommend using a 1 cell sector with a 3D-setup. A small non-zero swirl velocity at the axis can be then due to poor convergence.

Summary: do not use RSM for 2D axis-symmetric problems

Best regards, Amine

KgpNiko16 posted this 2 hours ago

Did you ran some test case yourself ?

I mean there are two paper

one is  "Reynolds Stress Model in the Prediction of Confined Turbulent Swirling Flow"  which uses fluent (most probably fluent 6) , simulates swirl flow using Axisymmetric swirl formulation , incompressible, steady , RSM and report results which is physically plausible and even validated.

and other is which is very much similar to my case Comparison of turbulence models in simulating swirling pipe flows also uses same type of formulation and this author  uses fluent 6.2 .

so is it the problem with higher version ? There is some kind of setting for axis which is hidden ?

KgpNiko16 posted this 52 minutes ago

How to make 1 cell thick 3d geometery ,is there any easy way out in Fluent ? Are you talking about  revolve mesh ?

When i revolve mesh there will be a large aspect ratio cell near axis . right ?  will that be a problem ?