May 3, 2021 at 10:47 amag1991Subscriber
I am currently simulating a case where a check valve is present. I would like to obtain as an output from my simulation the flowrate decrease as a result of valve closure.
The point is, the gap is about 10 microns and refining the mesh on this gap area makes the simulation becoming unfeasible, as the elements number increases beyond my computational capabilities.
I wonder if there is any tutorial regarding this kind of clearance flows that could help me, furthermore, I have heard some folks talking about manipulating the dynamic viscosity of cells in gap so the flow becomes restricted through that clearance, keeping at the same time a limited number of elements. Is this last procedure possible? Are there any examples available related to this kind of problem?
ThanksMay 3, 2021 at 1:43 pmKarthik RAdministratorHello What is the overall size of your domain and how does this compare with the 10 micron size you intend to mesh? Also, what gap ranges are you investigating? What is the Reynolds number of your flow at the inlet? To obtain a reasonable flow rate through a 10 micron gap, you will need an enormous pressure head?
Regarding meshing this, you could perhaps create a body of influence region around this valve and create a finer mesh here? This should help you create a local volumetric mesh refinement. There are multiple YouTube videos showing the BOI mesh.
May 3, 2021 at 2:14 pmag1991SubscriberThanks for your reply, Karthik.
The overall size of the domain is about 40 cm length where a few duct branches are present. On one of these branches (2 cm diameter) there is a check-valve which is used to prevent backflow.
Gap ranges are 1mm, 0.5 mm, 0.1 mm and 0.01 mm. There are big differences on leakage flowrate from case to case. To sum up, let's say you end up with 30%, 18% and 10% of the valveless case flowrate with each of these gaps, excluding the 10 microns case, which I am still managing to simulate.
As you mentioned, a huge pressure head will be required to force any leakage through this 10 microns gap, pretty much more than in any of the other cases. They key here is obtaining an almost zero flowrate with a 10 microns gap.
Reynolds ranges from 2000 up to 8000 (pulsatile flow) .
Of course, I have applied some BOI in order to refine the mesh on the gap area. This works fine for all cases but for the 10 microns one, where the number of elements becomes too large to go ahead with it. This is why I was asking if there is any procedure/best practice for these leakage flow case where it would be possible to manipulate gap cells viscosity so with a coarser mesh and greater gap the leakage becomes almost zero. To my knowledge, I am aware there is some people who have done something like this but I would like to know if there was any documentation or ideas available on this.
May 3, 2021 at 4:01 pmRobAnsys EmployeeYou could try porous media, but that's also using the solver to tune the solution. Otherwise sub models may work, or use a bigger computer: not everything can be solved on a desktop.
May 3, 2021 at 5:32 pmag1991SubscriberThanks Rob which kind of sub-models do you refer to?
These simulations have been launched on a cluster. I mean, the difference between a 10 microns and a 0.5 mm gap is too large in terms of elements, (about 40 Million cells if keeping the refinement only on the gap area), I am just trying to see if there are others who have already faced this kind of problem and if they managed to overcome this issue by using any other approaches.
Porous media could be another way to proceed, but that's conditioning my solution and what I actually would like to get from ANSYS Fluent is the flowrate and pressure drop.
May 4, 2021 at 1:25 pmRobAnsys EmployeeA sub model would be to model only part of the system. So, lose most of the valve geometry and model only a section of the valve gap. You can then correlate dP with flow.
May 13, 2021 at 5:01 pmag1991SubscriberRob, that seems a nice idea.
So far, I have tried a kind of different thing, I'll explain myself:
I have conserved all geometries in the model (including the valve)
I have activated Contact Detection option on Dynamic Mesh Settings, thus creating porous media for all fluid zones which lay under the geometric tolerance I've told you before
I am trying to simulate with the 6-DOF solver the closure motion for this valve and hence the activation of the porous media areas once it reaches the closing position
However, knowing how challenging it can be to achieve the full motion closure (with smoothing and remeshing), I have decided to generate a mesh where the check valve is closed and porous media are enabled, so I can test if the simulation is going to work or not. I am using Pressure Inlet and Pressure Outlet BC, but it seems its diverging for some reason. I don't know if restricting almost totally the flow through the check valve branch (and at the same time letting it flow through other branches) can't be admisible on a fluid simulation. Honestly, I don't know to what extent Fluent can manage such flows through narrow passages.
Would it be possible to simulate it with an overset mesh and using a collar mesh? This way I believe the check valve could overlap the proper walls of the duct, thus enclosing the flow.
Thanks in advance
May 14, 2021 at 9:30 amRobAnsys EmployeeOverset will work providing you have enough resolution to avoid orphan cells as the surfaces come into close proximity.
Using pressure in and pressure out means the flow rate becomes part of the solution: this can make convergence very dependent on the initial conditions so the model may be more unstable than you'd expect.
June 16, 2021 at 11:32 amag1991SubscriberHi Rob, since I am not able to apply at all the 'contact detection' feature, I am now trying to create the porous zone in the gap area in a similar way it would be created through 'contact detection' by following the next steps:
I create cell registers based on boundary distance corresponding to the zones where I would like to apply a porous media
Then I separate cells by marks based on those cell registers, so for instance, if i had before Zone 1 now it becomes Zone 2 and Zone 3, where Zone 3 is the zone region where I would like to apply the porous media
The point is, if I am right, the imposition of a porous media requires the creation of mesh-interfaces between porous zone and the surrounding zone (in this case between Zone 3 and Zone 2). But when I separate cells by marks, I don't get any mesh-interfaces at all. In fact, interior-cells are split into different boundaries, but I cannot convert these interior cells into interface type to create the mesh-interface.
Is it really mandatory to create mesh-interface between fluid zones when using porous media?
Would it work well the submodel by creating the porous media this way?
June 16, 2021 at 4:23 pmRobAnsys EmployeeYou're creating an interior zone, not an interface: there's a difference. You do need an interior as the porous zone is a separate cell zone.
June 17, 2021 at 3:12 pmag1991SubscriberSo in this case there is no need to actually create any mesh-interface between Zone 2 (standard flow) and Zone 3 (porous media). In fact, I have checked on a different simulation how 'contact detection' actually does not create any mesh-interface when creating a porous media.
Could you please tell me if there was any tutorial available regarding the phenomenon of 'flow blockage' through the use of 'contact detection' and 'flow control' features to assign a porous media to the region within a proximity threshold between two walls and hence virtually blocking flow through it? Like in the case of a narrow gap.
At this point, I am seeing some difficulties on converging the continuity residuals, as the sudden appearance of this porous media that sinks momentum seems too agressive. I am wondering if there are some guidelines when facing this situations.
June 17, 2021 at 3:59 pmRobAnsys EmployeeNot that I'm aware of. If changes are rapid the usual approach is to reduce the time step. may know more as it's something that may crop up in the FSI work.
June 21, 2021 at 11:21 amag1991SubscriberYeah, I agree with that Rob, although let me specify that in this case I am obtaining the check valve pure rotational motion through the use of 6DOF solver.
June 22, 2021 at 10:53 amRobAnsys EmployeeIf it's purely rotational (ie a ball valve) put the ball into one mesh and the valve into the other. Use an interface and you can rotate the valve section using sliding mesh. You will need to stop the motion and adapt as you reach fully closed to maintain some resolution but otherwise it's a normal use of the models.
June 22, 2021 at 3:26 pmag1991SubscriberUnfortunately this is not the case Rob. It requires the motion of two disks that almost touch each other. Nevertheless, the problem would be the same, the creation of that porous media to model the flow through the gap and its convergence instability issues.
June 22, 2021 at 3:29 pmRobAnsys EmployeeHave a look at the results, you may find you're not resolving the gradients sufficiently. Adaption may be a better option as you can refine just the region of interest rather than larger parts of the domain as you would with the more usual refinement approaches.
June 23, 2021 at 8:03 amag1991SubscriberI'll give it a try. I've also tried to patch (just before the porous media is created) the region upstream from the valve, where the pressure is meant to rise due to flow decceleration, with higher values for static pressure, zero velocity and k and omega, in an attempt to put things easier to the solver to converge to the actual pressure drop values once the porous media is activated. Unfortunately, this hasn't worked at all. I wonder if such procedure (that can be modified, be it by changing the patched values, be it by patching also the downstream region) has been performed by someone when facing this kind of problem. I mean, I believe a CFD case involving flow through small gaps on check valves must have been deeply studied since a few years, as check valves are commonly found on industrial applicatons.
June 23, 2021 at 8:21 amaitor.amatriainSubscriberCould you post some information about the topic that you mention related to the increase of viscosity?
Apart from the solutions proposed by and I can think of no alternative to solve your flow with maximum accuracy.
If you do not have not enough computational resources, you could try to create gaps of different sizes (of course, bigger than 10 microns) and then obtain the desired quantities in each of these cases. Based on the obtained results, you could make correlations and estimate the output in the 10 micron case.
June 23, 2021 at 10:17 amag1991SubscriberAitor, I am afraid the sources are not official at all, these simply are comments from some folks and unfortunately there is no written documentation, articles or tutorials referring to this idea.
One of the options suggested that taking advantage of the use of an overset mesh, the exact 10 microns gap could be simulated. The problem comes first from the unfeasible cell count, (meshing in fractions of that 10 microns size can make the mesh become too large), and then, you have great disparity of flow scales (ranging from the duct diameter of 2 cm to the 10 microns gap), I see this quite hard to handle by the solver itself. Therefore, this option is discarded.
Your idea regarding the correlation of results is good, but the draback is you'd be trying to extract a flow/pressure law from different geometries. On the other hand, the use of a porous media that can imitate the pressure drop at the gap region may prove to be the most accurate solution, in my opinion. Unfortunately, the appearance of such porous media makes the convergence quite difficult to attain.
Viewing 18 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.