September 27, 2017 at 11:19 amadminAnsys Employee
How to separate the inflation into a separate cell zone in Fluent?
October 17, 2017 at 7:53 amArun KumarSubscriber
Problem/Description: For MDM problems, it can be advantageous to separate the inflation layer into a separate cell zone. Doing so will allow you to have different MDM settings for the inflation layer than the surrounding elements. 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.
April 26, 2020 at 5:10 amvishwatejakasojuSubscriber
April 26, 2020 at 3:43 pmKalyan GoparajuAnsys Employee
This post should help you with what you are looking for.
- You must be logged in to reply to this topic.
- 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
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.