[Bisht]

Hi, I am doing the multiphase Simulation (Petrol and air) of a fuel pipe during filling process. To simulate the foaming formation in pipe I am using Euler-Euler Large scale interaction model. During Simulation, residuals converging for few time steps and then diverging very sharply.
I set Under relaxtion factors to the lowest value and refined mesh size but still this Problem persists.
Is there an error with my model or boundary condition?

I am using velocity inlet, time step= 10^-4
no. of inner Iteration= 25

[me3840]

Your timestep seems too big to me. What is the CFL of the fluid?

Please post pictures of your mesh?

[Bisht]

I am assuming CFL no = 1, based on this I got time step of 10^-4.
Velocity of fluid at Inlet is 4.158 m/s
total no. of cells around 0.7 millions

[Bisht]

In between, I tried to simulate it with a time step of 10^-5 but residuals are still not converging.

[me3840]

Yes, but what does the CFL actually look like in the domain during computation, i.e. was your estimate correct?

I expect lowering the URFs will just make you need to take more inner iterations to converge timesteps.

It can be hard to start transient cases like this since even small timesteps don't really model the startup physics correctly.

I would think, however, for a case like this you would want to use a VOF model rather than EMP, correct?

[Bisht]

In the Expression Report type, there is no CFL no. field function to choose. I couldn't see it there.
The main Task of my work is to simulate the pre mature shut off (PSO) of fuel nozzle. During normal filling it happens because of the foam and bubble formation in pipe due to entrapped air. I don't know where VOF can capture this behaviour effieciently or not, that's why I am doing it with EMP. Can we capture PSO with VOF?

[me3840]

There is a field function for convective courant number. You can also make a CFL field function if you want.

Hmm. I would suspect you could capture that with VOF, but yes, the simulation will be very expensive.

[Bisht]

I tried to run Simulation after creating the CFl no. Report and Monitor plot but it showing an error that couldn't evaluate field function convective courant number.
Yeah I am Aware that it's very expensive and time consuming.

[me3840]

What did you use for the report? You just need to make a maximum of convective courant number..

[devesh.baghel]

Hi,

1. What is the max CFL you are getting into your simulation ?
2. Did your try with VOF & Trimmed mesh ?
3. Are you modeling evaporation into your simulation ? If yes, what about the piezometric pressure ?
4. I hope you might have considered gravity and surface tension effect to capture near wall behavior......


Regards

[devesh.baghel]

Also check the location of Higher TKE & SDR of adblue.....do some refinement over there....

[Bisht]

Yeah I chose Gravity and surface Tension model. I didn't tried VOF as I am not sure that it can capture pre shut off behaviour of nozzle.
I changed the temporal scheme to first order and it's showing better results. Residuals are still diverging but after 4000 iterations. i think I Need to refine the mesh

[Bisht]

I created a scalar Scene and selected convective courant number as the scalar function. It's showing me CFL in range of 0.0085 to 33.
During analytical calculation I took cfl as one and on base of that calculated the time step but Simulation result is giving something else.
Does it mean that time step size of 10^-4 is too big for this Simulation?

[devesh.baghel]

Hi Kamal,

1. Did you find the location & at what time, divergence occuring ?
2. Start with less time step than current one, leter once fluid reached zone where recirculation,bubble formation, bends etc is absent, can increase time step slowly.
3. EMP model is better suit than VOF
4. Concentrare on Max CFL in whole domain and try to contol near to 1.
5. How are you checking PSO ?
6. Try "Trimmed Mesh" if time permits

Regards

[Bisht]

Hi

Divergence occuring around 0.015 s. CFl no. for the domain changing insanely during simulation reaching as high as 10^5.
I am using a fine mesh in the area of high speed flow with a maximum size of 0.8 mm, time step is already 10^-4 ´, I chnaged it to 10^-5 but CFL for the domain is still high.
for the wholedomain CFL no is 1 or less than one it's getting high at a corner but that point is above my inlet. Among all the parameters TKE of Adblue (same as water) is getting diverge sharply. Other parametrs seems reasonable.
I attached a scalar scene of cfl no.

[me3840]

Your mesh from your previous pictures isn't shown that high, but I would take a look at your mesh quality. Compute the maximum skewness angle and see if you can get your prisms to stop collapsing all over the place; do they need to be so thick? Generally getting a skewness angle below 85 can be challenging poly+prism, but it is doable. Also take a look at volume change < 0.001 and cell quality < 0.1.

[Bisht]

Hi,
I checked mesh quality and skewness angle. It shows some problematic faces but everything is above inlet. Down the inlet where water flows is perfect. I tried trimmer mesher but it fails to capture curves of the domain properly and producing a very bad mesh. Prism layer getting colapsed beacuse I am using Advance layer mesher, it maintains the first prism layer thickness everywhere and drops the other layers if the gap is not enough to produce complete prism layer-

[devesh.baghel]

Hi Kamal,


1.Attached picture shown higher CFL might be because of local high velocity of gas. Please check the mesh as suggested.
2. Also need to reduce time-step atleast 10^-5 or less than that till exit of gas get becomes smooth i.e. till the fluctuation dampened out. after than slowly you can increase time-step with help of macro.

Regards