January 9, 2019 at 5:07 pmMohsenhivaSubscriber
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.
January 10, 2019 at 5:35 amKeyur KanadeAnsys Employee
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.
January 10, 2019 at 2:40 pm
January 10, 2019 at 4:00 pmRobAnsys Employee
Try reducing the timestep. You need the solver to run such that the valve cannot cross one cell in a timestep.
January 14, 2019 at 10:01 amMohsenhivaSubscriber
Thanks for your comment. I have still the same problem with time step 0.0001! What can I do?
January 14, 2019 at 11:20 amRobAnsys Employee
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?
January 14, 2019 at 3:41 pmMohsenhivaSubscriber
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.
January 14, 2019 at 6:47 pmDrAmineAnsys Employee
I encourage you to watch the first part of the tutorial shared by my colleague:
January 15, 2019 at 4:07 amKeyur KanadeAnsys Employee
in remeshing panel, please use mesh scale info and use those values in min and max length scales.
January 17, 2019 at 10:59 amMohsenhivaSubscriber
Thanks a lot. I did so. But no success yet!
January 18, 2019 at 3:50 amKeyur KanadeAnsys Employee
please refine mesh further reduce time step.
January 21, 2019 at 4:05 pm
January 22, 2019 at 3:26 amKeyur KanadeAnsys Employee
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.
January 22, 2019 at 1:22 pmMax4Subscriber
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.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- Exporting Data Results