ERROR: averaged velocity didn't match gas superficial velocity

Submitted by ljmutue on Wed, 10/03/2018 - 15:23

Dear All,
I am trying to simulate a small section of the dilute gas-particle flow in a riser.
The boundary conditions for the particle phase were set as periodic boundary in the z direction (boundary m m p). The solids volume fraction is 0.018.
The boundary conditions of incompressible gas phase are: uniform inlet boundary at the bottom (0 0 0.0925) and pressure outlet boundary at the top (zeroGradient). The other boundaries were set as no slip walls.
The solver is cfdemSolverPiso.
Based on an overall mass balance, the time and spatially-averaged velocity at different heights should be equal to the gas superficial velocity, which is 0.0925 m/s. However the time-averaged Ugz along the height is about 0.085 m/s, i.e. almost 10% smaller than the expected value (see Fig.1).

For solving this, I have tried the following:
1. Change tolerance and relTol in system/fvSolution to 1e-06 and 0 respectively;
2. Change different gas inlet boundary, from uniform inlet to flowRateInletVelocity or interstitialInletVelocity;
3. Change drag model from BeetstraDrag to GidaspowDrag.
After all these changes, the problem still remains.
Then I tried to empty the region, i.e. single gas flow without any particles. In that case the time-averaged Ugz in a large part of the bed is equal to the superficial gas velocity, whilst errors still exist in the first few grid layers from the bottom, as shown in Fig.2.

Does anyone ever meet similar problems? All your feedback would be highly appreciated.

The software versions are:
OpenFOAM: 5.x
LIGGGHTS: 3.8.0
CFDEMcoupling: 5.x

Thank you all for your help.
Kind regards,
Lijing Mu (TU Eindhoven)

AttachmentSize
Image icon fig.1.jpg16.8 KB
Image icon fig.2.jpg25.87 KB
cgoniva's picture

cgoniva | Fri, 10/05/2018 - 09:52

Hello Lijing Mu,

I have no answer, but questions which might help find the solution:

  • what BC did you use for voidfraction?
  • Did you check the flux at the inlet where you use fixed value velocity?
  • What is actually the flux field (please look up in the code you use what phi stands for - is it U*faceArea or U*faceArea*voidfraction?)

Here my suspicion: you might be using zeroGradient for voidfraction at the inlet which leads to not inserting the flux you want to. Given I am right you might consider using fixedValue 1 for voidfraction and see if you get the flux you like to see. If that solves the issue, you might think of using a more sophisticated BC for U so you can have zeroGrad for voidfraction and still the desired flux.

Please let me know your progess on this issue.

Best regards,

Christoph

ljmutue | Fri, 10/05/2018 - 13:43

Hello Christoph,

Thanks so much for your reply.

The definition of phi in the code I use is U*faceArea*voidfraction.
I have tried both fixedValue 1 and zeroGradient for voidfraction. Under both these two conditions, the flux is around 0.086 (lower than expected 0.0925).
Do you mean the more sophisticated BC for U is type flowRateInletVelocity or interstitialInletVelocity? If so, I have tried these two types for U and zeroGradient for voidfraction, however the flux is still lower than expected.

When I remove all the particles and only gas flow left in the domain, BC I use for U is fixedValue uniform (0 0 0.0925) and BC for voidfraction whether fixedValue 1 or zeroGradient wouldn't matter in this condition, there are wiggles exist in the first few grid layers from the bottom (attached file Fig. 2). Do you have any thoughts why this would occur? Any help would be very much appreciated!

Kind regards,
Lijing

ljmutue | Thu, 03/14/2019 - 11:04

Thanks Christoph,

Based on your feedback, I solved this problem.
I'll upload the solution here:
step 1. set fixedValue 1 for voidfraction at the inlet;
step 2. set fixedValue 0 for Ksl at the inlet;
step 3. set fixedFluxPressure bc for all patches except outlet.

After these settings, the averaged velocity should match the superficial gas velocity. Problem solved!

Kind regards,
Lijing

yirenxindudu | Wed, 09/11/2019 - 10:17

how to add interstitialInletVelocity in CFDEM?
inlet
{
type interstitialInletVelocity;
inletVelocity uniform (0.00015 0 0);
value uniform (0.00015 0 0);
phi phi.air;
alpha alpha.air;
}
what should be replaced by alpha.air?