[hitzhwan]

When I simulate the gas-liquid flow with VOF model, it always divergence，is the mesh problem ？ Do I need dense the mesh in the gas-liquid interface? I try to use mesh adaption, but it does not work, it make the case divergence more quickly. How can I solve the problems？

[CFDKareem]

Divergence with the VOF model is *almost* always caused by too large of a time step. Make sure the CFL number is not going above 1 for the interface. Courant = velocity(time step/mesh length) for VOF.

[hitzhwan]

Originally Posted by CFDKareem

Divergence with the VOF model is *almost* always caused by too large of a time step. Make sure the CFL number is not going above 1 for the interface. Courant = velocity(time step/mesh length) for VOF.

Hi，but for the coupled scheme, the default CFL is 200, should I set it 1?

[CFDKareem]

Originally Posted by hitzhwan

Hi，but for the coupled scheme, the default CFL is 200, should I set it 1?

Are you running a transient simulation?

[hitzhwan]

Originally Posted by CFDKareem

Are you running a transient simulation?

Yes，that is right.

[CFDKareem]

Originally Posted by hitzhwan

Yes，that is right.

Ok, then the Courant number you want is dependent on your time step and mesh size. The Courant number under the coupled scheme is different, and you can disregard it for now. You can approximate the multiphase Courant number by hand, or use adaptive time stepping. If you use adaptive, you can set the global Courant number to 1 and fluent will adjust the time step automatically to achieve the set value.

The Courant number, for multiphase, can be thought of as how fast the interface between the two fluids moves across the mesh. Ideally, the interface will only move <1 mesh elements per timestep. For more complex simulations the number can be relaxed to 3-5, but usually at the cost of accuracy.

[hitzhwan]

Originally Posted by CFDKareem

Ok, then the Courant number you want is dependent on your time step and mesh size. The Courant number under the coupled scheme is different, and you can disregard it for now. You can approximate the multiphase Courant number by hand, or use adaptive time stepping. If you use adaptive, you can set the global Courant number to 1 and fluent will adjust the time step automatically to achieve the set value.

The Courant number, for multiphase, can be thought of as how fast the interface between the two fluids moves across the mesh. Ideally, the interface will only move <1 mesh elements per timestep. For more complex simulations the number can be relaxed to 3-5, but usually at the cost of accuracy.

Thank you so much,but I have three questions for you:

1)so you mean the Courant number under the coupled scheme does not have any function, it real Courant number only depends on the time step and mesh size, is that right .

2)In addition, you provide me a useful method to use the adaptive time stepping, but that have a problem.Because I need monitor the data by the time step, if it is adaptive tiem stepping, I cannot process the data by known flow time, how to solve this problem?

3. If it always divergence and I want to use the fixed time step, and the boundary condition has no problem, does that mean the only way is to change the mesh model make it more available? How can I decide it?

[CFDKareem]

Originally Posted by hitzhwan

Thank you so much,but I have three questions for you:

1)so you mean the Courant number under the coupled scheme does not have any function, it real Courant number only depends on the time step and mesh size, is that right .

2)In addition, you provide me a useful method to use the adaptive time stepping, but that have a problem.Because I need monitor the data by the time step, if it is adaptive tiem stepping, I cannot process the data by known flow time, how to solve this problem?

3. If it always divergence and I want to use the fixed time step, and the boundary condition has no problem, does that mean the only way is to change the mesh model make it more available? How can I decide it?

1) It does have a purpose, but in your case the default setting should be okay. The Courant number you care about is only dependent on mesh size and time step.

2) you can you a fixed timestep, but have to make sure it satisfies the Courant <1 condition throughout the whole simulation. It will add some time to the calculation, but should be okay

3) You are correct that you have two parameters to change: mesh size and time step. The mesh size should be set according to the physics and simulation problem. The mesh should be fine enough to capture the physics of interest, but not too refined that your time step has to be ridiculously small. I would recommend starting with a coarse mesh, and therefore larger time step, to check your initial simulation. If you're error is too high, then you can go back and refine further.

[hitzhwan]

Originally Posted by CFDKareem

1) It does have a purpose, but in your case the default setting should be okay. The Courant number you care about is only dependent on mesh size and time step.

2) you can you a fixed timestep, but have to make sure it satisfies the Courant <1 condition throughout the whole simulation. It will add some time to the calculation, but should be okay

3) You are correct that you have two parameters to change: mesh size and time step. The mesh size should be set according to the physics and simulation problem. The mesh should be fine enough to capture the physics of interest, but not too refined that your time step has to be ridiculously small. I would recommend starting with a coarse mesh, and therefore larger time step, to check your initial simulation. If you're error is too high, then you can go back and refine further.

Thank you so much.

1） What is the detail purpose?

2) I set 1e-5 fixed time step which can assure Courant <1 initially, but it abruptly divergence on the calculation progress, how to solve it?

3) Do you find a strange phenonmen, when I do the mesh independency study, when I refine the mesh number, the results always change a lot (about 5% deviation) and made my time step very small, have you met this problem, how to solve it?

[CFDKareem]

Originally Posted by hitzhwan

Thank you so much.

1） What is the detail purpose?

2) I set 1e-5 fixed time step which can assure Courant <1 initially, but it abruptly divergence on the calculation progress, how to solve it?

3) Do you find a strange phenonmen, when I do the mesh independency study, when I refine the mesh number, the results always change a lot (about 5% deviation) and made my time step very small, have you met this problem, how to solve it?

1) See this thread for details: Fluent Courant Number Value ?!!

2) You probably need a lower timestep. As stated eariler, the fixed timestep has to cover the entire simulation. So as your fluid accelerates the Courant number will increase as well. At 1e-5 it is probably okay for the intial stages of flow, but not so much as the flow develops.

3) The timestep decreasing with refined mesh makes sense. The change in error is a complex thing to pin down. There can be a lot of sources of error, not just the mesh. If changing the mesh is not changing the error, then it is likely coming from another source (Boundary conditions, numerical model, etc.)

[hitzhwan]

Originally Posted by CFDKareem

1) See this thread for details: Fluent Courant Number Value ?!!

2) You probably need a lower timestep. As stated eariler, the fixed timestep has to cover the entire simulation. So as your fluid accelerates the Courant number will increase as well. At 1e-5 it is probably okay for the intial stages of flow, but not so much as the flow develops.

3) The timestep decreasing with refined mesh makes sense. The change in error is a complex thing to pin down. There can be a lot of sources of error, not just the mesh. If changing the mesh is not changing the error, then it is likely coming from another source (Boundary conditions, numerical model, etc.)

1. Thank you for your sharing.

2. My timestep is 1e-5, if I lower it to 1e-6, the calculation time would be too large to burden, how can I solve it?

3. I find the another sources have no problem, but the results change with the increasing of mesh numbers, it will not reach steady until one mesh number, what is the reason? Have you met this problem?

[CFDKareem]

Originally Posted by hitzhwan

1. Thank you for your sharing.

2. My timestep is 1e-5, if I lower it to 1e-6, the calculation time would be too large to burden, how can I solve it?

3. I find the another sources have no problem, but the results change with the increasing of mesh numbers, it will not reach steady until one mesh number, what is the reason? Have you met this problem?

2) Yeah that is the challenge with the VOF model. Your only option is to increase the mesh size, but if you need it small to capture physics then you'll have to deal with the small timestep to maintain accuracy. I have had VOF models that require 1e-8 or less for parts of the simulation, sadly.

3) I am unsure of exactly the problem you are having. I would need to know more about what your setup is and what variables you are tracking.

[hitzhwan]

Originally Posted by CFDKareem

2) Yeah that is the challenge with the VOF model. Your only option is to increase the mesh size, but if you need it small to capture physics then you'll have to deal with the small timestep to maintain accuracy. I have had VOF models that require 1e-8 or less for parts of the simulation, sadly.

3) I am unsure of exactly the problem you are having. I would need to know more about what your setup is and what variables you are tracking.

1)How long does it take you to calculate for the case with 1e-8, have you tried the adaptive mesh function, can it help your case? When I use the adaptive mesh, it may lead disvergence, what is the reason?

2)I mean the mesh independency study, the variable can be any you want ,it is just to make sure the calculation model is accurate with the mesh model.

[CFDKareem]

Originally Posted by hitzhwan

1)How long does it take you to calculate for the case with 1e-8, have you tried the adaptive mesh function, can it help your case? When I use the adaptive mesh, it may lead disvergence, what is the reason?

2)I mean the mesh independency study, the variable can be any you want ,it is just to make sure the calculation model is accurate with the mesh model.

For my work I prefer a fixed mesh, but use adaptive time stepping to help speed up the simulation. Even through the timestep is variable, I set up an automatic export of the data at a consistent time step. These models can take anywhere from 2-24 hours to solve depending on the mesh density and exact physics being tracked. The total time modeled in my work is usally around .01 seconds.

[hitzhwan]

Originally Posted by CFDKareem

For my work I prefer a fixed mesh, but use adaptive time stepping to help speed up the simulation. Even through the timestep is variable, I set up an automatic export of the data at a consistent time step. These models can take anywhere from 2-24 hours to solve depending on the mesh density and exact physics being tracked. The total time modeled in my work is usally around .01 seconds.

“I set up an automatic export of the data at a consistent time step. ”，but the time step is not fixed, how can you process the data in flow time?


How many mesh number do you have for the 1e-8s time step, it only take less than 24 hours? What is parameters for you pc?