TAGGED: #fluent-#cfd-#ansys, fluent, mesh
May 16, 2023 at 3:37 pmJeroen PouwelsSubscriber
First of all, I want to mention that I am a complete rookie when it comes to Ansys. I did some FEM analyses for my studies, but I am completely new to doing CFD simulations using it.
I am doing my bachelor assignment on air bearings and I am currently trying to run CFD simulations using Ansys Fluent for the air flow through a sliding air bearing. However, I do not seem to be able to get an accurate or correct volume mesh (see picture). The bearing has three inlets: two on the side and one in the middle. The one in the middle will need the highest inlet pressure since it needs to carry most of the weight of the object sliding through the bearing. The two side inlets are mainly for balance. I specified the outer edges of the rectangular parts as the outlet since this is where the flow will go into the environment again. From there, the flow's parameters are not of interest anymore. I included my solidworks assembly of the air bearing and the sliding mass going through it as well as my Design Modeler model of the volume where the air can go (see grey area in the picture as well) using a WeTransfer URL at the end of the post.
I was wondering if anyone could help me with creating a good mesh and setting the model up for a simulation. Thanks in advance!
May 16, 2023 at 4:16 pmFederico Alzamora PrevitaliSubscriber
are you using any of the Fluent Meshing workflows? Also, what are the errors highlighted in your image? Self-intersections? Overlapping faces?
May 18, 2023 at 9:09 amJeroen PouwelsSubscriber
Hi Federico, I indeed use Fluent Meshing Watertight Geometry workflow. I believe it is overlap, so my main question at the moment comes down to how to mesh this very thin (10 micron) layer of air and how to mesh the air channels below it without creating overlap.
May 17, 2023 at 7:18 amNickFLSubscriber
I am having difficulty visualizing it at that angle. Pehaps you could show the geometry a better picture with some descriptions of where the BCs are, etc. Do you need or want to use Fluent Meshing or can you use ANSYS Meshing? Typically air bearings are very thin in one direction so it is useful to decompose the geometry to obtain a high quality hex mesh with high aspect ratio elements. Simply using a “tet-bomb” approach will result in too many elements. Are you going to include mesh motion in your simulation? These are all important things to consider before undertaking such a project.
Welcome to the world of CFD:)
P.S. Most of us cannot download files from random sites. Please make images (and marked up images are even better) and post them here. ANSYS has created this nice forum that hosts these pictures quite well.
May 18, 2023 at 9:22 amJeroen PouwelsSubscriber
Hi Nick, thanks for the reply. I thought it would be best to use Fluent Meshing for this, but I am completely open to suggestions. I added a better image regarding the geometry of the volume as well as an image of the bearing itself. I hope this makes it easier to visualize. The outlet is marked red, the middle inlet is marked blue and the side inlets are marked green. Every other face is selected as the wall.
It seems like you know how to mesh the thin airflow between the slider and the bearing as well as the airflow channels underneath. Could you maybe explain more thoroughly how you would approach that? The airflow between the slider and bearing is 10 microns thick and the channels have a diameter of 1 to 2 mm, but I will start with 1mm.
May 18, 2023 at 11:11 amNickFLSubscriber
My recommendation would be to do this in ANSYS Meshing. Read up on body decomposition and multibody parts in ANSYS.
If I were to create it, I would create several bodies for the inlet tube network (I don't think they are all connected are they? I think I see three independent paths.) and then a mutli-body part for the thin air channel. You could create this in such a way that you would not have to go back and remesh when you are in a different position from the nominal. Instead, you would simply scale the mesh to adjust the dimensions. The downside to this approach is, you would not have a congruent mesh (1:1) at the tube/channel interface, but you could use a finer mesh to have the interface approach be effective.
May 18, 2023 at 11:27 amJeroen PouwelsSubscriber
Okay, thank you, I will switch to that then. What I did now is I created the three bodies for the tube networks and I created a fourth body for the thin layer of air. The only thing I adjusted to the standard mesh is the addition of inflation layers for the tubes. I am currently trying to add an inflation layer for the thin layer as well but that gives the following error messages:
- The inflation layer generation did not complete. This may be due to poor quality patches in the surface mesh, sharp geometric features, or narrow passages.
- Patch conforming mesh failed possibly because of bad boundary or inflation mesh.
- A mesh could not be generated using the current meshing options and settings.
I also added some pictures of how it looks now
Would you suggest any other edits to the standard mesh for the piping system? And how do you suggest that I mesh such a thin layer?
Thanks for your help already!
May 18, 2023 at 11:36 amNickFLSubscriber
The thin air channel will not mesh well with tets -- especially with tets the sizing it is trying there. The body looks simple enough to sweep/multizone, but I would cut it up further so that you could have a resolved mesh where the inlet come in.
As for the piping network, I would try and see if you could use multizone to mesh these. Then you could have more high aspect ratio hex elements to reduce your mesh count.
May 19, 2023 at 10:47 amJeroen PouwelsSubscriber
Hmm where do you suggest I cut it up? Also, when trying to use multizone with hex elements for the piping I get the following error: MultiZone blocking decomposition failed.
Do you know what this means?
May 23, 2023 at 6:18 amNickFLSubscriber
See below for a simple example. I would have something like this around each of the holes. The inner circle should be bigger than the max deviation of the feeder pipes. There should also be at least 6, probably 8 or even better 10 layers through the thickness (into and out of the screen). The mesh sizing here is too coarse, but I wanted to demonstate the idea.
May 23, 2023 at 8:46 amJeroen PouwelsSubscriber
Ooh, I see what you mean now, thanks. After cutting it up, what meshing methods did you use here then?
May 23, 2023 at 10:54 amNickFLSubscriber
Those are all 6-sided blocks, so the sweep works well. You can put sizing on all the edges with biases and everything to really control the mesh.
May 23, 2023 at 11:36 amJeroen PouwelsSubscriber
Okay, thanks. I will try it later today!
May 19, 2023 at 11:09 amRobAnsys Employee
Slicing and dicing geometry is a bit of an art form, and one that's not been practiced much for several years. Have a look at the various meshing courses, and read up on Sweep (Ansys Meshing). Multizone is going to struggle becuase of the pipe orientation connecting into the model from multiple directions (y & z).
May 23, 2023 at 11:37 amJeroen PouwelsSubscriber
May 23, 2023 at 10:55 amNickFLSubscriber
Is that your way of saying that I am old?
May 23, 2023 at 2:08 pmRobAnsys Employee
No comment! ;) Given I learnt to fully block mesh (single block, none of this multi-block stuff) with cartesian cells I'm not sure what that would make me.... I prefer experienced!
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.