CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Fluent Multiphase (http://www.cfd-online.com/Forums/fluent-multiphase/)
-   -   Diffusive interface in VOF model (http://www.cfd-online.com/Forums/fluent-multiphase/121618-diffusive-interface-vof-model.html)

jd113 August 1, 2013 09:30

Diffusive interface in VOF model
 
1 Attachment(s)
I am trying to simulate droplet flow in a small 2-D slit. For this I have introduced a small inlet into the channel. Flow of primary phase,water(red,see image) is on both sides of the channel; the dispersed phase toluene(blue is coming through the inlet.

I have used these settings: second order schemes for all including time, PISO and implicit scheme with 1e-8 cutoff. Mesh is in mm (0.15x0.25 mm inlet) with 10 micron quad mapped cells. I start with first order scheme and then after first iteration revert to second order.

My flow rates are of 4mm/s, time step is 1e-7 , flow is purely laminar and Courant number is not a problem. The continuity criterion are all 10^-8 with only vf-phase criterion 10^-6.
I have worked with finite elements and I have known the over-diffusive effects of second order terms in hyperbolic flows. I am new to finite volume but I doubt such large diffusion can be caused by it laminar flows. I am struggling to understand this diffusive spreading of the interface. From looking at the mass conservation given in FLUENT manual it seems that this spreading can occur only if there is a source term which is set to zero by default. In this case the mass in and mass out should cancel and nothing should move out. I am baffled by this spreading.

Any suggestions will be useful. Thanks.

Jabba August 2, 2013 09:06

the diffusive behaviour that you are getting is due to the application of the second-order upwind (I assume) scheme for discretizing the volume fraction transport equation

due to the discrete nature of the interface, special interpolation schemes are required in order to capture a sharp boundary between the phases

when using a implict time formulation, it is recommended that you use HRIC or Compressive schemes

in a explicit time calculation, the Geo-reconstruct method is most commonly applied

hope it helps



Quote:

Originally Posted by jd113 (Post 443296)
I am trying to simulate droplet flow in a small 2-D slit. For this I have introduced a small inlet into the channel. Flow of primary phase,water(red,see image) is on both sides of the channel; the dispersed phase toluene(blue is coming through the inlet.

I have used these settings: second order schemes for all including time, PISO and implicit scheme with 1e-8 cutoff. Mesh is in mm (0.15x0.25 mm inlet) with 10 micron quad mapped cells. I start with first order scheme and then after first iteration revert to second order.

My flow rates are of 4mm/s, time step is 1e-7 , flow is purely laminar and Courant number is not a problem. The continuity criterion are all 10^-8 with only vf-phase criterion 10^-6.
I have worked with finite elements and I have known the over-diffusive effects of second order terms in hyperbolic flows. I am new to finite volume but I doubt such large diffusion can be caused by it laminar flows. I am struggling to understand this diffusive spreading of the interface. From looking at the mass conservation given in FLUENT manual it seems that this spreading can occur only if there is a source term which is set to zero by default. In this case the mass in and mass out should cancel and nothing should move out. I am baffled by this spreading.

Any suggestions will be useful. Thanks.


jd113 August 3, 2013 05:49

Thanks. The simulation is now running well with explicit Geo reconstruct.


All times are GMT -4. The time now is 06:10.