August 8, 2018 at 11:16 pmElhussienSubscriber
Hello Karthic, thanks
attached are some screenshots
the boundary conditions are quite simple :
1- inlet : zero velocity air inlet.
2- all the sides are zero pressure outlets.
3- the drop is set on the surface where a contact boundary layer is expected.
the rest are set as default
it was initialized "hybrid"
August 8, 2018 at 11:44 pmKarthik RAdministrator
I have moved your question to a different thread so you will be able to find more help.
You might perhaps want to test out a 2D problem using the VOF. You could attempt a 3D case once you get your desired solution for the 2D problem. This will help you debug your simulation and understand the VOF set-up.
You might want to set-up a problem similar to the physical formulation in the figure above. You might want to create a simple rectangular domain and use 'Patch' initialization and 'Mark' a circular region identifying the liquid drop. You might want to run a transient Explicit VOF simulation on this problem. Please ensure you set-up your wall contact angle under the wall boundary conditions panel. Please make sure you have defined your surface tension (similar to the way you are doing from the Interaction panel). Air would be your primary phase and water secondary.
Couple of thoughts on your current set-up:
- Please use a conformal mesh for your model. You will not have to deal with 'Mesh Interfaces' in Fluent. It becomes much simpler to set-up the model. Please have a look at ANSYS how to videos to understand creating conformal mesh.
- Please use a transient model.
- Please also show what conditions you are using for all your boundaries and highlight them. This will help us clarify your boundary conditions.
I am also attaching an excellent VOF tutorial by Raef Kobeissi here for your help.
I hope this helps.
August 9, 2018 at 9:29 pmElhussienSubscriber
Thanks Karthik for everything
let me to say that I don't find a sub routine to enter the contact angle.
Also I tried the Ink-jet tutorial before but it's not related, the same with spray cooling cases.
I will work on the 2-D model I used to perform 3-D only and will discuss the results.
August 9, 2018 at 9:38 pmKarthik RAdministrator
You do not need to run a sub-routine for specifying static equilibrium contact angle. You can do this from the wall boundary condition panel. Make sure you have 'Wall adhesion' checked from the 'Phase Interaction' panel. You will be able to specify the contact angle from the wall boundary condition panel. Please see the screenshots below.
Regarding ink-jet nozzle application: I totally agree with you that the problem you are solving is different from ink-jet nozzle application. However, it is an excellent place to start learning VOF set-up in Fluent.
I hope this helps.
August 10, 2018 at 7:33 amDrAmineAnsys Employee
Do you need to apply a dynamic contact angle based on a certain correlation or theory? Then you need UDF. Several researchers claim that one does not need the dynamic contact angle as it is a result of proper well resolved VOF run. Others however are persuaded that a prescription of dynamic contact angle is a must (advancing and receding angle based on local flow/properties/what ever).
The DEFINE macro you require is then DEFINE_PROFILE
August 13, 2018 at 4:25 pmElhussienSubscriber
Thanks bro for being concerned
I discuss the matter of contact angle with my supervisor and he think that it should be dynamic contact angle
I run the 2--D Case and it resulted that the circular drop still circle; i.e it's not flattened!!
August 13, 2018 at 5:13 pmKarthik RAdministrator
Could you please post some transient images / animation of your volume fraction contours? Please post VF contours at initial time t = 0 and then at various subsequent time intervals. This will help us understand your issue. I am suspecting there is some issue with your simulation set-up. Please post appropriate images so we can help you better.
August 26, 2018 at 6:02 pm
August 26, 2018 at 7:12 pmKarthik RAdministratorHello
If these contours are not changing with time, I am pretty sure there is an issue with your model set-up.
Did you activate gravity in your model? Is the vector in the right direction?
What surface tension formulation are you using - CSF or CSS?
Are you using an implicit and explicit VOF formulation? What is your time step? What is your Courant number?
How long did you run your simulation for?
Could you please explain your boundary conditions in your model?
Did you activate ‘wall adhesion’ from the interaction panel? And are you able to specify a contact angle from the wall BC panel? What is your value?
Please answer these questions in as much detail as possible so we can understand your model and help you move forward in your simulation.
August 26, 2018 at 10:07 pmElhussienSubscriber
1- yes it doesn't changed with time.
2- Yes I activate the gravity in my -ve Y direction.
3- CSF model .
4- Explicit VOF, with 0.01 second time step and (0.25) Courant number.
5- For 300 time steps and Max. iteration/ time step=1.
6- B.C :
a) zero velocity inlet air velocity i.e in water multi-phase I entered that the volume fraction with zero.
b) the upper boundary is a wall.
c) the lower boundary is a contact with 90 degree as in the attached .
August 26, 2018 at 11:20 pmKarthik RAdministrator
Thank you for this information. Here are some suggestions:
- Please make sure you are converging every time-step. Please increase the maximum number of iterations per time-step to 20. This will allow the solution to achieve the desired convergence residual criteria set. This is important for a transient problem.
- Also, please make sure you have sufficiently low time-step such that the Courant number is close to 1 or lower. You can read more about this in the Fluent Users guide.
- Also, you do not need to use a velocity inlet boundary condition. Please refer to my image from a previous post. You can use pressure outlet on all three ends (with 0 backflow VF of water, similar to the way you set-up).
Please make these changes and let me know your findings.
September 17, 2018 at 10:17 pm
September 18, 2018 at 1:28 amKarthik RAdministrator
Please follow the steps based on my previous response and make sure you are converging every time step. Please share a screenshot of the residual plot here. Please make sure you are reaching the residual criteria you have set for your problem.
Also, could you also let us know what your time step size is?
Please run your simulation with a pressure outlet condition on the three sides, with back flow enables.
Please let us know what you find.
September 20, 2018 at 8:37 pmElhussienSubscriber
Here is the result based on your recommendations;
my time step is 0.001 sec., Courant number is 1 and all sides are pressure outlets.
As shown from the screenshot; the solution is converged every time step.
The main difference between this result and the last one is that the final contour of water volume fraction for the drop is zero while it was 1 when the inlet was velocity inlet boundary condition.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.