"reversed flow in ### faces of pressure outlet"

  • 509 Views
  • Last Post 14 December 2018
  • Topic Is Solved
lucaavv posted this 07 December 2018

Hi

I'm trying to simulate an horizontal rotating disk on which will flow water, I have made the fluid domain and the mesh.

For the solution I'm using VOF model without change and the k-epsilon RNG with swirl flow added. I have made the mesh that have

minimum orthogonal quality equal to 0.7 but i'm having problem because I have the message "reversed flow in ### faces on pressure

outlet". For some iteration it converge at 1e-3 and than it stop converging as the number of faces on which the flow is reversed as grown

up. I'm using time step between 1e-3 and 1e-6 with Curant number equal to 1.5.

1) How can I solve the reversed flow problem?

2)How can I improve the mesh for the cylindrical geometry?

3)Are the models rigth for what I want to simulate?

Order By: Standard | Newest | Votes
kkanade posted this 07 December 2018

Please refine mesh further and decrease timestep size.

lucaavv posted this 10 December 2018

Thank you for your suggestion but i hoped to use another way.....

Did someone have another suggestion?

 

rwoolhou posted this 10 December 2018

Please can you post images of the model?  Reversed flow tends to mean the outlet is too close to the area of interest, or that the flow is swirling near the outlet. It may not matter to the solution, but without seeing the model I don't know. 

If the liquid is spreading on the disc and then atomising as it's thrown off you will need a high cell count to capture the free surface breaking up. What are you trying to model? 

lucaavv posted this 10 December 2018

Hi and thank you  for reply,

I'm trying to model a rotating disk of 1mm thickness and 10cm diameter, I have divided the disk in thinner disk to improve the mesh, the bonduary condition are

pressure outlet=1 atm for the lateral surface, shear stress=0 for the top wall and moving wall with rotation speed=60 rps for the bottom. I have water inlet      

(velocity inlet=5m/s) in a 1 mm diameter tube( 5e-6 height) in the center of the highest disk.

 

I have uploaded the project in drive if you are interested in watching it

https://drive.google.com/open?id=1bUsdDFTUAYFRYl29ygZjFxMhD3KNJnvQ

 

thank you

rwoolhou posted this 11 December 2018

I can't download the case as ANSYS staff are not allowed to. 

However, what I think is happening is water enters and flows across the plate. Water then leaves at the circumference. Water probably doesn't occupy the whole volume so air is moving in/out on the circumference. There's a good chance you don't have enough mesh in the axial direction, and potentially around the inlet. 

With 5m/s in a 5 micron height you're looking at a time step of   (cell height/speed)/10    ie a lot smaller value than you have used.

You also need to note that the wall shear and surface tension force gradients will be very high so you'll to carefully monitor the solution: we typically don't model much below 50-100 microns as things get very interesting. 

Assuming you're using Fluent you could use a 2d axi-symmetric model to do this model: it'll drop the domain volume so you can use A LOT of cells to make sure you pick up everything. This will further decrease the time step but means it's more likely to work. 

 

lucaavv posted this 11 December 2018

Thank you

I can't use a 2d model because I'm interested in the film thickness and whole fluid behaviour, i wil try to improve the mesh near the cirumference and in the axial

direction and i'll let you know how it goes.

Regarding to the mesh in the axial direction I have divided the fluid domain in thinner disk with the "slice by plane" command, have you any suggestion of

other method for improve the mesh?

rwoolhou posted this 11 December 2018

Merge all of the sliced volumes together. If you're sweeping the mesh you can slice the model into sectors. Having done this you can set edge biasing on all of the axial edges: you can then cluster cells towards both walls. Adaption may also be an option: this means you can subdivide cells as needed to track the free surface. 

 

lucaavv posted this 12 December 2018

 For now I have tryed to improve the mesh near the periphery by creating an anular region with very thin element and I have also increased the value at

pressure outlet surface and it seems to work, I still have the reversed flow message but it is going up with iteration. I'll also try different solution

Thank you

rwoolhou posted this 12 December 2018

That may be the correct solution. The liquid fills in the centre, at the perimeter it's separated from one of the walls and there's a gas layer that penetrates some distance into the domain. 

lucaavv posted this 12 December 2018

A last question, at the upper surface I have made the condition wall with shear equal to 0, is that right or a better condition would be another pressure outlet?

The shear was for the liquid-gas interface, but the fil thickness is much lower than the domain I have used.

How does FLUENT see this fact? He have a wall with shear=0(that is like air) in contact with air

 

rwoolhou posted this 13 December 2018

A pressure inlet or outlet would be more suitable, and set the back flow to "from neighbouring cell" and air as the material. 

Using a wall means any liquid that hits the surface will be constrained. If you find water is hitting the pressure increase the height of the domain as it means you're constraining the result. 

 

lucaavv posted this 14 December 2018

Thank you

 

Close