Learning Forum

[Mohsenhiva]

Dear friends,

I am willing to simulate a check valve to confine the pressure from a water hammer within an air vessel. In fact, as you can see in the following images, a valve at downstream creates water hammer. I have air in the air vessel. I want that after a water hammer see the surge pressure entering the air vessel. The check valve is supposed to let flow only in +y direction. The problem is that check valve doesn't move at all. Do you have any comment on this?

Thanks a lot. 

[Keyur Kanade]

from image, dynamic mesh settings look ok. you may want to click off layering option. 

can you please simplify problem. can you please reduce mass, remove spring constant and check. 

https://www.youtube.com/watch?v=Va6aI96UDj0

 

[Mohsenhiva]

Dear kkande,

 

Thanks for your advice. I did so. This time the check valve moves upward. But, the simulation stops due to a negative mesh error. I think I must reduce the movement speed of the check valve. Do you have any suggestion? 

 

[Rob]

Try reducing the timestep. You need the solver to run such that the valve cannot cross one cell in a timestep. 

[Mohsenhiva]

Thanks for your comment. I have still the same problem with time step 0.0001! What can I do?

[Rob]

OK, then check your remeshing settings: do you have remeshing turned on? If so, check the size/skew settings to make sure they'll pick up the cell sizes you're using. 

What is the cell size, and how fast is/can the valve move?

[Mohsenhiva]

The element size is 0.002 m and I used triangular cells with 5 inflation layers. Regarding the remeshing, yes it is turned on. I put a screenshot from the remeshing window. Thanks for your time. 

For the valve, I don't control the velocity of movement it is supposed to move based on the change in pressure force on it similar to a real-world case.

[DrAmine]

I encourage you to watch the first part of the tutorial shared by my colleague:

 

https://www.youtube.com/watch?v=9-Tu-Koy-D8

[Keyur Kanade]

in remeshing panel, please use mesh scale info and use those values in min and max length scales. 

[Mohsenhiva]

Thanks a lot. I did so. But no success yet!

[Keyur Kanade]

please refine mesh further reduce time step. 

[Mohsenhiva]

I reduced the time-step and refined the mesh in the check valve zone. But still, I have a negative mesh problem! Any more suggestion, please?

 

 

[Keyur Kanade]

the mesh looks weird at the shoulder. the inflation layer is abruptly stopped. looks like you have different cell zones at that edge. 

you may want to use a single cell zone. 

[Max4]

You can create another cell_zone for the inflation layer around the valve. In the dynamic mesh settings, set this cell_zone as Rigid Body so that this layer moves with the valve. This can be done around the wall too.

An example of its usefulness is a falling rigid object in a fluid domain. If the rigid object is represented as a void in the mesh surrounded by an inflation layer, and the elements surrounding the inflation layer are tet elements, then separating the inflation layer will allow you to specify rigid body motion to the inflation layer (so that the inflation element quality is maintained throughout the simulation) and remeshing/smoothing is only performed on the surrounding tet elements. Solution: There are two ways to separate the inflation layer. 1) If the inflation has a constant # of elements: Adapt > Boundary > Option = Cell Distance > Number of Cells = inflation layers > Boundary Zone = [wall boundary with inflation] > Mark > Mesh > Separate > Cells > Mark > Registers = Marked Zone > Separate. 2) If the inflation elements are a different element type than the rest of the mesh: Initialize > Adapt > Iso-Value > Iso-Values of = Cell Info… > Cell Element Type > Compute > Mark separate zone for, e.g. element type 6, which is triangular prisms. Separate marked zone as above.

 

Regards,

Maxime