April 29, 2021 at 9:09 amTE_HafSubscriber
The problem I am trying to simulate involves the machining of a material, where I want to simulate the fluid flow induced by the rotation of the tool.
Is it possible to use a sliding mesh around the rotary tool, and make it slide over a wall?
For example, if I have a disk saw, the teeth will be in direct contact with the wall. The contact point will slide a little bit every time step, but still be in contact with the wall.
Is this possible with the sliding mesh method, or is a minimal gap necessary (such as is needed when using MFR)?
This was not clear in the user guide.April 29, 2021 at 12:26 pmKarthik RAdministratorHello Yes, I don't see why you cannot solve the model using the sliding mesh approach. You will have a stationary (material being machined) and a rotating zone (the tool, I suppose). The RPM is going to be relatively large (I presume)? Make sure you have a good mesh and the same mesh resolution on both sides, especially around the interface.
MRF might have the advantage of making the flow field steady (again, I don't know the exact problem you are solving, but something to think about) relative to the moving reference frame.
April 29, 2021 at 2:31 pmTE_HafSubscriberHi yes, it is a straight plate, that is going to be machined with a milling cutter with approx. 5000 RPM.
The problem with MRF is that I need to have a small gap, so that the interface is not on the wall. That increases the mass flow and modifies the streamlines because there is a continuous flow between tool and workpiece. That flow changes the flow inside the milled channel.
The goal is to use a method where there is no gap. Do you think this method works if the slinding interface is located at the wall of the workpiece?
I tried using the overset mesh method, but could not get rid of Orphan cells, that would lead the simulation to diverge.
May 2, 2021 at 3:36 pmRobAnsys EmployeeIf the sliding interface is at the wall you will need to be careful with fluid/solid interactions (and how you define the zones) but it should work.
May 6, 2021 at 7:31 amTE_HafSubscriberHi,
now that I started working with the geometry there are some things that are not clear to me.
The mesh at the tool side is only within the teeth of the disc saw (when created using designmodeller), resulting in several bodies (the number of bodies is the number of empty spaces between the teeth).
I probably need to define surface meshes between the teeth following the curvature of the circle and at the sides of the blade where I can impose the no-slip condition (the wall of the tool that rotates), right?
On the fluid side, I will probably also have some places where there is only a surface mesh, and not any fluid, so that I can define them later as walls, otherwise they will be missing, right?
May 6, 2021 at 8:58 amTE_HafSubscriberAn update:
1- Created surface bodies (shells?) for the walls of the disc saw, grouped in a part, and named them as wall
2- Created surface bodies for the walls of the workpiece/air part
3- When exporting the mesh to fluent, the surface bodies disappear (no volume associated?)
That resulted in more questions:
A: Why are the surface body meshes not visible/available in fluent?
B: While trying to define an interface in fluent, I have a combination of fluid interfaces (gaps between teeth) and walls (surface bodies, that are not there, problem above...). Should I have one large surface (disc) for each part (sliding and not sliding) that incorporates all the intersections, and smaller surfaces for the separate parts (wall, fluid) where I can apply boundary conditions?
Here follows a picture of the disc saw: Gray is the wall (solid body), also interface solid-fluid and red is the fluid, also the interface fluid-fluid.
Thanks in advance!
May 6, 2021 at 10:51 amRobAnsys EmployeeFluent 3d requires solid (fluid) regions and doesn't recognise surface geometry: it does recognise faces that make up the volumes. With a circular tool the other problem is that the tool only touches at a point, that's going to cause problems with the mesh in that region, so you may need to tweak the geometry slightly whilst retaining the circular interface. This could mean an overset approach is needed, with some care where the blade penetrates the workpiece.
May 6, 2021 at 11:42 amTE_HafSubscriberThank you,
I think this also answers the first question. It will not work when there are discontinuous wall contacts.
What I meant with a "gap" was fluid between the tip of the tool and the interface. Without this gap the interface is made of wall surfaces (tool) and fluid surfaces (fluid between teeth). With the gap there is at least one layer of fluid cells to avoid direct contact between the wall of the workpiece and the wall of the tool.
I tried using the overset mesh approach previously, but the same wall-wall contact generated orphan cells, which caused the solution to diverge. I think this would be another discussion.
May 6, 2021 at 11:56 amRobAnsys EmployeeYou can have solid:solid either side of an interface so could create a slight dip in the workpiece to reduce the sharp angle where the tool makes contact.
May 6, 2021 at 12:33 pmTE_HafSubscriberBut how would it be for the other 270 degrees of the saw that are in contact with the fluid?
May 6, 2021 at 12:40 pmRobAnsys EmployeeThe saw will still interact with the rest of the fluid zone: you model the "outside" in one domain and the "blade+gaps" in the other. The latter is fully enclosed by the former.
May 6, 2021 at 1:52 pmTE_HafSubscriberSorry, I am not sure if I understood it right. Adding some 2D drawings to the discussion:
The setup is a disc saw grooving a workpiece:
The computational setup (let's say it is in 2d):
The black lines show the size of the fluid domain (air), with the lower lines representing the workpiece. Red is the interface between tool and the background, blue is the fluid between the teeth of the saw.
1- There is a curved surface missing where the wall would be, fluent does not allow me to add just a surface and define it as wall there, because there is no fluid. So, the rotating zone is not completely inclosed.
2- The red interface can be moved closer to the teeth, so that it will be solid-fluid-solid-fluid... and so on, or away from the teeth so that it is only fluid. The second approach will increase the gap between the teeth and the workpiece.
The depth of the groove varies between 3-10 mm, while the size of the disc saw is about 150 mm. If I want to model the flow in the groove, a gap, depending on the size can change the fluid flow in more than 50%.
For it to work, two gaps are necessery, one at the tool side and one at the workpiece side, otherwise there will be no volume cells at the curved part of the workpiece.
I could not understand how can I have solid:solid at the interface, while it is rotating.
May 6, 2021 at 5:04 pmRobAnsys EmployeeCreate a thin solid region where the metal would be at the bottom of the domain. Black will be walls & red is an interface. Model the blade as a solid too as this gives you something to attach the interface too. It's one of those situations where you model the solid zone purely to hang boundary conditions onto it.
May 7, 2021 at 10:48 amTE_HafSubscriberNow that makes sense! I will give it a try.
May 21, 2021 at 12:33 pmTE_HafSubscriberHi,
I had the time to change the geometry and mesh and start some simulations and check if it works.
I still have some questions regarding the setup:
a) The solid workpiece is in contact with the fluid body. I created an interface with the coupled walls setting. Is that OK? User guide says that where there is no interface between 2 faces a wall boundary condition is assumed.
b) The interface between the fluid within the saw teeth and the fluid within the larger domain was set with the matching option, since the mesh was not perfectly matching. Is that OK? It seems to work at least during initialisation.
c) The interfaces create additional surfaces, that are automatically added to the walls group. Should I change that to moving wall, rotation, and leave the rotation value empty, or should I use the same rotation value I am assigning for the solid disc saw (Body 1) and the fluid between the teeth (body 2) in the cell zone conditions? That was not clear.
I checked some tutorials, and the tutorial for the centrifugal fan uses a moving wall setting for the blades(walls), although the blades are already part of the moving mesh cell zone. The rotation velocity, however, is left empty, and only filled in the cell zone panel. Should I leave it emtpy (0) or use the same value as for the cell zone?
d) I am having a problem, on the first fluid cells of the large fluid domain, right where the interface with the saw is located. If you look the previous figure, it the thin region right where the red circle is tangential to the black line. Right before this region I have a solid body, that creates the boundary between the surface of the workpiece (left side) and the surface at the bottom of the groove (lower line on the right).
I am not sure if this is caused by the thin elements at this region, or by the contact between solid and fluid. Here is how the mesh looks like:
Unfortunately, that results in a velocity 100 times larger than possible, leading the AMG solver to diverge. Should the solid piece be larger, so that there is some contact with the wall BC at the bottom of the groove?
May 21, 2021 at 1:00 pmRobAnsys EmployeeThe walls are to cover where the interface doesn't line up: from memory just leave them alone.
The issue with the fluid region is because of the sharp corner. Either thicken it a bit or trim a bit off the end: I suspect the skew in that area is excessive.
Matching is covered in the manual, it shouldn't do any harm and is more related to geometry matching over mesh.
June 7, 2021 at 11:46 amTE_HafSubscriberHi I made some changes and played a little bit with the setup, and came across something that is not clear to me.
I set the tool (solid, moving at 500 rad/s), the fluid between teeth (fluid, also moving at 500 rad/s), the surrounding air (fluid, stationary) and the workpiece(solid, stationary).
If I initialize the case and plot the velocity at the plane where the interface with the wall should be (the red zone where the tool, in white, is in contact with the side wall of the groove), instead of v=zero (because it is a stationary wall) It returns a value as high as the tangential velocity at the given radius (see below the red region).
So the air within the teeth of the saw is rotating, but was initialized like everything else, without velocity. I confirmed that looking at a cross section and at the symmetry plane.
These planes also show something weird.
The velocity at the tool interface is the tangential velocity (OK) and decreases to zero, but the velocity at the workpiece has the same red contour, although it shoud be stationary.
Has this something to do with the fact that the rotating tool is in direct contact with the workpiece? Is it not possible to have free-slip at the solid-solid contact. while no-slip at the fluid-solid contact?
If one thinks from the perspective of the control volume within the teeth of the saw it would look like a moving wall. The velocity , hovewer, would be opposite to the velocity of the control volume in the absolute frame. In the absolute frame, the control volume moves, but I still would expect a gradient at the wall, otherwise there would be no influence of the wall (slip-free).
June 21, 2021 at 8:43 amTE_HafSubscriberSo to answer my own questions:
Fluent creates non-overlapping faces. Those faces correspond to the regions where additional boundary condition can be set.
The region in red in the previous post (where a wall should be located) is the non-overlapping face of the sliding mesh. Therefore it requres a moving mesh BC, where the absolute rotation is zero, or, where the rotation relative to the adjacent cell zone is -500 rad/s.
The non-overlapping region adjacent to the non-sliding domain has the shape of the tool (visible in white in the previous post), and therefore needs to be defined as a moving wall, where the absolute rotation is 500 rad/s.
This way it presents the correct BCs at the initialization.
With the BCs for the non-overlapping zones the solid parts (tool, workpiece) are not necessary.
Viewing 17 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
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- 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.