Result of my simulation is different when the momentum discretization scheme is changed

  • 248 Views
  • Last Post 17 July 2018
  • Topic Is Solved
banitabaei posted this 25 June 2018

I have a simulation for impact of a droplet onto a particle (axisymmetric vof). 
I have created my Case an I need to study effect of droplet viscosity on impact outcome. So, I use the same case every time, but I change the liquid phase properties on it. As I increase the droplet viscosity, formation of the liquid film due to impact is getting hindered (which is expected based on the physics of the impact). However, as shown in Fig. 1, there is a return point for this behavior (happens around mu=10 cP) which is not expected (although there are papers reported a similar behavior which hinders liquid 'splashing' around the same viscosity mu=10).

Initially, I use '2nd order upwind' for the momentum equation. As shown in Fig. 1, when I changed it to QUICK, there is a significant difference between the results for mu=10 (as far as I know, QUICK is mostly good for the structured mesh, while I'm using unstructured).

Does anyone know which one of these solutions I should rely on?

Thank you

 

Order By: Standard | Newest | Votes
Kremella posted this 28 June 2018

Hello,

This is what Fluent theory guide has to say about QUICK.

For more information on which scenarios to use these discretization types for, I would recommend you go to the Fluent Theory Guide .

However, this does not explain the behavior.

Best Regards,

Karthik

  • Liked by
  • konangsh
abenhadj posted this 28 June 2018

You have to ensure for deep convergence on both cases before starting a consistent comparison. QUICK will lose it superiority compared to SOU whenever you are not using structured meshes.

 

Kind regards,

Amine

Best regards,

Amine

raul.raghav posted this 28 June 2018

I'm quite confident that something has gone wrong in the setting up of the Second-Order Upwind case for 10cP droplet viscosity (look at the image below). Your droplet spreads well at both 0.65cP and 5cP viscosity values, and then for the 10cP value, it seems like the droplet is approaching the obstruction at a significantly lower velocity compared to the other cases and encapsulates the obstruction. Something doesn't sound right here and I'm sure it has to do with the setup.

QUICK provides a better accuracy on quadrilateral and hexahedral (structured) meshes and by default it applies the Second-Order Upwind scheme on unstructured meshes. Refer: Spatial Discretization and Other Discretization Schemes.

Rahul

banitabaei posted this 01 July 2018

Thanks for everyone's response. The velocity is the same in all cases and I've checked it many times. Even I've run the simulation for mu=9 and 11 and it came out that the change happens smoothly.

However,  I realized that the reason I'm getting different results for mu=10 in the original question that I asked is related to whether I use implicit or explicit volume fraction formulation (it's apparently not related to QUICK or 2nd oredr). The reason is that I made a small change in the 2nd order simulation (which was originally explicit) and made it implicit, and the lamella was formed in mu=10.

I know the implicit methods are sometimes considered to be more reliable since they are iterative. I think, if I decrease the time step in the explicit method. it will probably give me the same results as the implicit method.

Is there any preference in terms of which solution I should consider being more accurate here? Any ideas are greatly appreciated.

 

Thanks

 

Kremella posted this 02 July 2018

Hello,

Thank you for your update.

You are correct, implicit formulations are iterative and explicit are non-iterative. However, if you are solving a transient problem, I'd recommend you use an explicit formulation as opposed to implicit. It tends to show better numerical accuracy when compared to implicit for time-dependent solution. Here is what the Users Guide says (section 24.2.2, v18.2)

Choosing volume fraction formulation

In addition to this, implicit scheme tends to be numerically diffusive (especially with first order transient formulation) compared to explicit.

I hope this answers you question.

Best Regards,

Karthik

  • Liked by
  • banitabaei
  • konangsh
banitabaei posted this 03 July 2018

Thanks for the note.

In my initial explicit solution, I used a variable time step with Courant Number CN=0.2

- Based on your response above, going forward I'm going the to use explicit method. I think I need to decrease my CN to decrease the time step. How should I find the proper CN for these simulations?

- Another thing which is still not very clear to me is what kind of mesh works better here. In my initial solution, I used triangular mesh. Should I keep using that or better to move to hexa while I'm using the explicit method? (I've attached a picture of my mesh to show the density of cells in the domain. It's hexa mesh though). Since I'm going to finalize the setup, any other comments regarding the mesh or the parameters in the case file would be really helpful and appreciated.

Kremella posted this 03 July 2018

Hello,

I tend to prefer using a structured mesh always compared to an unstructured. It tends to reduce the overall grid size of the simulation. This tends to be of very high importance for 3D simulations (not so much for 2D). I understand that it might not always be possible to created structured grids. It is, however, extremely important to have meshes with low-skewness (especially when using explicit schemes). These are some thoughts based on my limited multiphase flow modeling experience.

One comment about your mesh: I like the fact that you have tried to gradually refine your mesh in the interfacial regions. This should improve the accuracy of your solution. Good luck with your modeling!

Thank you.

Best,

Karthik

  • Liked by
  • banitabaei
  • konangsh
banitabaei posted this 03 July 2018

Thanks very much! 

A few more points for clarification:

1- Could you please give me a clue regarding what criteria to use for choosing Courant Number (for variable time steps)?

2- The only issue with explicit is that I can only use '1st Order' for the "Transient Formulation", while with the implicit method, I can choose a 2nd order. Is it okay?

3- For pressure, momentum, and volume fraction, is there a particular method that you can recommend for this specific problem (for instance, between 2nd order, QUICK, and 3rd order MUSCL) or for different methods available for volume fraction (i.e. Geo-Reconstruct, CICSAM, Compressive, and HRIC).

4- Should I use Coupled Level Set + VOF (CLSVOF method) here?

5- I've attached detailed pics of my setup below. I'd appreciate if you have a look and let me know if you think anything else needs a modification too (I understand that there might be no definite answer for some of them, I can try two better options and choose the best one based on the results). I just wanna make sure nothing is wrong before I run this simulation several times and get results.

Thanks for responding to the posts regularly and in detail as they become a great resource for the future users.

abenhadj posted this 17 July 2018

Hi,

1/As small as possible for accurate results but this would cause some overhead. A global of one or two in the case of explicit VOF interpolation is fair enough. 

2/Explicit does only allow for First Order Backward Euler scheme

3/Geo-Reconstruct and Compressive are the schemes which we recommend. For Transient runs with small time step you can start with PISO

4/Just carry out a sensitivity analysis

A.

Best regards,

Amine

Close