Dynamic Mesh or Overset Mesh for a moving objects in a flow domain when we have small gaps?

  • 193 Views
  • Last Post 05 March 2018
fardinkhalili posted this 17 January 2018

Hi,

I want to do a simulation for a bileaflet mechanical heart valve. Initially, the geometry has very small gaps like 0.05-0.1 mm in the hinges. The pulsatile fluid flow through the valve and leaflets rotate around their hinges (1DOF). During the backflow the leaflets closes the flow domain and prevent the backflow. The movement of the leaflets are not predefined and they move based on the pulsatile flow.

Questions:

1. Should I choose the dynamic mesh approach or overset mesh?

2. What should I do for the small gaps since the small flow with higher stresses inside the hinge (small gaps) are also important?

3. What criteria for the meshing should I consider if I want to have LES as turbulence models

Thanks.

Order By: Standard | Newest | Votes
saadyw posted this 07 February 2018

Hi 

could you attach a sketch for more understanding ?

fardinkhalili posted this 08 February 2018

I did simulation using 1-way coupling Fluent and transient structural.

My question is now:

This a mechanical heart valve simulation in which the leaflets rotate about 55 degrees around their hinges to fully close the flow domain.

I run the simulation from fully-open position for a while so that the flow gets stable and then the leaflets are allowed to rotate. I have improved the simulation using Dynamic mesh option (smoothing diffusion parameter 1 and 2, layering height ratio and default parameters, and remeshing local cell, face and region remeshing). Now the leaflets rotate up to the last angles and simulation diverges before the leaflets and valve close.

The skewness angle is less than 0.65 at the beginning but the mesh cells get compressed and stretched to get skenewss angle of 0.96.

How to prevent this much deformation in the mesh?

vganore posted this 08 February 2018

Hi Fardin, you need to play around with re-meshing parameters and time step size (use smaller time step). Looks like your cells are not getting re meshed well when it exceeds max and min length scales. Also, in which region cells skewness is going beyond .96? Have you assigned any motion to leaflets?

Vishal Ganore, ansys.com/student

  • Liked by
  • fardinkhalili
fardinkhalili posted this 08 February 2018

Hi Vishal,

 

The leaflets are moving (known rotation from transient structural coupled with Fluent) from 0 angle to 55 degree.

Yes, It seems that remeshing is not doing anything as you see the mesh is streched at the center and compressed between the leaflets. I am using Local Cell, Local Face, Region Face for remeshing methods, Sizing Function is NOT on. I set the Minimum and Maximum Length Scales from the Mesh Scale Info and set the maximum cell skewness and face skewness to 0.85 and size remeshing interval is 1.

The highest skewness angle is 0.7 before running and get higher than 0.96 in regions: 1. mostly between the leaflet tips, 2. leaflets and wall on both sides.

 

vganore posted this 08 February 2018

Have you assigned any motion in transient structural? what is your motion equation? I wish to know the reason behind using transient structural. With using UDF in Fluent, you might get good control.

Do you have uniform mesh all over your fluid domain. If no then using mesh scale info on meshing parameters may not work. Please share your project file achieve. Let me investigate. 

Vishal Ganore, ansys.com/student

fardinkhalili posted this 08 February 2018

Yes the motion is assigned to the leaflets in transient structural based on a table including time and rotation angle. The reason is just doing the 1-way coupling as an approach for this simulation. we have used dynamic mesh and overset mesh and similar problem occurs when the leaflets is closing.

I added body sizing and sphere of influence and increased the quality of the (smaller size) in the region around the leaflets. It means that from inlet to downstream of the leaflets have smaller mesh, and larger mesh elements for the rest of the flow domain (far downstream of the leaflets.

 

vganore posted this 08 February 2018

I suggest you to separate dynamic mesh affected region near the leaflet from main flow region and generate uniform mesh for leaflet region. This will help solver to correctly predict maximum and minimum length scale in a select region for remeshing. 

Is there any linear or non linear relation between time and rotation angle. If yes then define that equation through UDF in Fluent to cut down extra transient structural physics. 

Vishal Ganore, ansys.com/student

saadyw posted this 05 March 2018

Hi Fardinkhalili

I except that you should use sliding mesh (not dynamic). This approach allows you to enclose the leaflets by interfaces and assign them to rotate with the desired angle according to a udf. see sliding mesh section in the fluent theory manual.

Regards

 

Close