[amir2552]

Hello everyone,
I am modeling the capillary rise inside a tube.
I want to plot the position of the fluid front vs. time.
Or find the fluid front position in each time step.
I will be so pleased if you could help me.
Thanks

[vinerm]

The fluid-gas interface would not have a single position, so, either you can track average position or maximum and minimum values, as far as a single value is concerned. However, you can certainly track the evolution of the iso-surface of volume fraction 0.5 for liquid (or gas). This will show the animation of moving front. But this will not give you a plot of some value vs. time.

[amir2552]

Originally Posted by vinerm

The fluid-gas interface would not have a single position, so, either you can track average position or maximum and minimum values, as far as a single value is concerned. However, you can certainly track the evolution of the iso-surface of volume fraction 0.5 for liquid (or gas). This will show the animation of moving front. But this will not give you a plot of some value vs. time.

Thank you for your reply.
If I just want to know the fluid front element positions in each time step, how can find them.

[vinerm]

In Fluent, moving mesh is not used for interface capturing or tracking. The mesh is always fixed. The approach used is called VOF and it captures the interface using volume fraction occupied by a particular fluid. So, if you want to determine where the front is, you just need to create an Iso-surface of Volume Fraction of either gas or liquid with a value of 0.5. Then you can export the values of all coordinates on this front. However, this will not be a single value until and unless the front is planar, such as, if water is drained from a very small hole in a very large tank, then the water-air interface would be plane for quite a long time, except near the end of draining. Since you are talking about capillary, the front is certainly not plane. Hence, cannot be represented by a single value. Though you can use average coordinate to represent the front.

[amir2552]

Originally Posted by vinerm

In Fluent, moving mesh is not used for interface capturing or tracking. The mesh is always fixed. The approach used is called VOF and it captures the interface using volume fraction occupied by a particular fluid. So, if you want to determine where the front is, you just need to create an Iso-surface of Volume Fraction of either gas or liquid with a value of 0.5. Then you can export the values of all coordinates on this front. However, this will not be a single value until and unless the front is planar, such as, if water is drained from a very small hole in a very large tank, then the water-air interface would be plane for quite a long time, except near the end of draining. Since you are talking about capillary, the front is certainly not plane. Hence, cannot be represented by a single value. Though you can use average coordinate to represent the front.

Thanks for your complete description. Would you please let me know how can I create an Iso-Surface? and How can I extract the surface's position result from Fluent?
Thank you very much in advance.

[vinerm]

You can follow the link below for surface creation. It would available under Surfaces in ribbon in new versions.

For extraction, you can use File > Export > Solution. Select ASCII and then surface that you created.

[amir2552]

Originally Posted by vinerm

You can follow the link below for surface creation. It would available under Surfaces in ribbon in new versions.

For extraction, you can use File > Export > Solution. Select ASCII and then surface that you created.

Thank you Vinerm for your help. Can I create an Iso-surface (or iso-line) in a 2D model?
I can't find the link you provided.

[vinerm]

https://www.afs.enea.it/project/nept...ug/node885.htm

[amir2552]

Originally Posted by vinerm

https://www.afs.enea.it/project/nept...ug/node885.htm

Can I create an Iso-surface (or iso-line) in a 2D model?
Thank you

[vinerm]

Yes, this is doable. It will be a line, automatically.

[amir2552]

Originally Posted by vinerm

Yes, this is doable. It will be a line, automatically.

Do you know any method to automatically export data files in ASCII format?
thank you

[vinerm]

Fluent has it inbuilt. Use File > Export > During Calculation. Choose ASCII and setup the frequency. Do not export at every time-step.

[amir2552]

Originally Posted by vinerm

Fluent has it inbuilt. Use File > Export > During Calculation. Choose ASCII and setup the frequency. Do not export at every time-step.

I am using an automatic variable time step in my analysis, could you please let me know, how can I print every time step that was taken by Fluent? or the elapsed time after each time step.
(I want to plot flow front vs time, in the constant manual time step, I can connect the flow front location to the time but in variable time step I cannot find the elapsed time for each location)
Thank you in advance

[vinerm]

Whenever you enable Automatic Time-Stepping and auto-save with time-steps is enabled, Fluent automatically writes the values for time in the output file. However, while setting up autosave, you have to select flow-time instead of time-step. Furthermore, when Fluent is running, it reports time-step value after every time-step. So, you can pick-up those values from the log or out file, provided you saved it.

[amir2552]

Originally Posted by vinerm

Whenever you enable Automatic Time-Stepping and auto-save with time-steps is enabled, Fluent automatically writes the values for time in the output file. However, while setting up autosave, you have to select flow-time instead of time-step. Furthermore, when Fluent is running, it reports time-step value after every time-step. So, you can pick-up those values from the log or out file, provided you saved it.

Thank you for your help.
Do you know which Courant number should be suitable for this kind of analysis?

[vinerm]

If you are using Implicit VOF, then you can go up to a rather high value but should keep it below 10 for good results. For Explicit, it is limited to 1.99999.

[amir2552]

Originally Posted by vinerm

If you are using Implicit VOF, then you can go up to a rather high value but should keep it below 10 for good results. For Explicit, it is limited to 1.99999.

Hello Vinerm,
Could you please let me know, How can I define rectangular mesh shapes inside Ansys meshing.
For example, consider a rectangular Shape. Its length and width are 10 and 5.
I want to have rectangular meshes with length 1 and width 0.5. In this way, I will have 10 elements on each side.
Thank you

[vinerm]

You have to apply mapped meshing on Face. If you apply equal number of divisions on opposite sides, meshing will automatically create mapped mesh.