May 4, 2022 at 4:11 pmsnr1Subscriber
How the number of elements along the axial direction of the 3D cylinder can be controlled in ANSYS meshing? Kindly help me with the procedure for thisMay 5, 2022 at 9:45 ampeteroznewmanSubscriberUse a Mesh Method, Sweep. You can enter the number of elements along the sweep direction.
May 5, 2022 at 10:47 amsnr1SubscriberWill you please elaborate on it step by step? I am unable to get what you are suggesting.
May 5, 2022 at 8:23 pmpeteroznewmanSubscriberThe image you show looks like you are in Fluent. There are two places you can mesh: using Fluent Meshing and using ANSYS Meshing, which you specifically mentioned.
In Workbench, start with a Fluid Flow (Fluent) analysis system. Double click the Geometry cell and create the cylinder in SpaceClaim, then close SpaceClaim.
Now double click on the Mesh cell to open the Meshing software. Right click on the Mesh branch and Insert a Method.
Set the method to Sweep. Type in how many divisions you want.
May 6, 2022 at 10:45 amsnr1SubscriberThank you for your detailed steps. I tried the same procedure. But the following error has been encountered. How to deal further with this issue.
"One or more non-sweepable bodies have sweep method controls and cannot be swept."
Geometry details: Stepped cylinder (Small cylinder or nozzle diameter = 2.2 mm, 20 mm length and bigger cylinder diameter = 33 mm and 1000 mm length)
Meshing methods used: a. Method: Multizone b. Mesh sizing for small and bigger cylinder diameter, and c. Face meshing of bigger cylinder
The image is attached.
May 6, 2022 at 11:36 ampeteroznewmanSubscriberI did not see the nozzle in your first image. This makes that solid a non-sweepable body. The insructions below will cut that body up into 3 bodies, each of which are sweepable.
Open the geometry in SpaceClaim. On the Design tab, use Split Body to cut the nozzle off the cylinder. Hide the nozzle body. Sketch on the planar face of the cylinder a circle with the diameter of the nozzle. That will split the planar face into two faces. Pick the nozzle-sized face and use Ctrl-C, Ctrl-V to copy the face and paste a surface. Hide the surface. Use the Pull tool to pull the nozzle-sized face through the length of the cylinder. Unhide the surface. Use the Pull tool, select No Merge on the options. Click the surface, then use the Up To button (or type U on the keyboard) then click the other end of the cylinder. Now you have 3 bodies. Show all Bodies. On the Workbench tab click the Share button. Now the mesh will be shared at the coincident surfaces.
In the Meshing app, delete the Multizone control. Create two Sweep methods, one for the nozzle and one for the cylinder with the hole in it, since they each want a different number of elements along the sweep direction. The long nozzle-sized body inside the cylinder will automatically follow along with the mesh on the larger cylinder with the hole in it.
May 6, 2022 at 4:19 pmsnr1SubscriberThank you for your procedure. If you don't mind, kindly can you share any tutorial on this method?
May 9, 2022 at 1:32 pmpeteroznewmanSubscriberI forgot one step, at t=4:14, click on the Workbench tab, click on the Share button and click on the green check to create Shared Topology to get shared nodes on coincident faces between bodies.
May 9, 2022 at 3:15 pmsnr1SubscriberThank you, peteroznewman. That's great work and help from you
Viewing 8 reply threads
Ansys Innovation Space
- The topic ‘Number of elements along the axial direction of a 3D cylinder’ is closed to new replies.
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.Trending discussions
- Floating point exception
- How to indetify baffles in Fluent meshing
- How to delete elements on Ansys Workbench
- Meshing cylindrical bodies with holes
- Quality failure limits are exceeded on some solid bodies… in ansys meshing
- Problems in the meshing of my geometry
- Ansys Mechanical – Python Scripting – Access and input parameter
- Fluent Meshing Batch Mode – Problems workflow commands
- Local mesh refinement with targeted edge lengths at specified areas
- Mesh Element Quality Display Style Not Showing
Top Rated Tags
© 2023 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.