CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > ANSYS Meshing & Geometry

[ICEM] The ICEM Guide for CFX Users

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes
  • 5 Post By JuPa
  • 1 Post By JuPa
  • 1 Post By Batis

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 28, 2015, 09:51
Thumbs up The ICEM Guide for CFX Users
  #1
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
I’d like to create a guide for CFX users who use ICEM. I’d like some clarification from ICEM power users to help clear this age old issue.

CFX Recommendations for Mesh Quality

In the CFX modelling guide, the suggested measures of mesh quality are:
  1. Mesh orthogonality
  2. Mesh expansion
  3. Mesh Aspect ratio

Mesh Orthogonality

The concept of mesh orthogonality relates to how close the angles between adjacent element faces or adjacent element edges are to some optimal angle (for example, 90 for quadrilateral faced elements and 60 for triangular faces elements). The most relevant measure of mesh orthogonality for the CFX-Solver is illustrated below. It involves the angle between the vector that joins two mesh (or control volume) nodes (s) and the normal vector for each integration point surface (n) associated with that edge. Significant orthogonality and non-orthogonality are illustrated at ip1 and ip2, respectively.



There are 6 orthogonality measures:
  1. Orthogonality Angle

    Large values indicate good orthogonality, and this must be more than 20.

    In ICEM I think this is called
    • Min ortho
    • Max ortho

  2. Orthogonality Factor

    Area weighted average of all integration point surface scalar products associated with each control volume.
    Must be more than 1/3.

    Unclear what the ICEM equivalent is

  3. Orthogonality Angle Minimum

    Same as point 1, but the minimum value. Must be more than 10

  4. Orthogonality Factor Minimum

    Same as point 2, but the minimum value. Must be more than 1/6.

    Unclear what the ICEM equivalent is

  5. Minimum/ Maximum Face Angle

    CFD-Post only. Must be between 10 and 170
    Must check your mesh in CFD Post to get this value.

    I don’t know if ICEM has an equivalent criterion.

  6. Minimum/ Maximum Dihedral Angle (ANSYS ICEM CFD)

    Must be between 10 and 170
    This is the only criteria where the CFX modelling guide refers directly to a mesh criteria in ICEM

Notes: the criteria for points 5 and 6 are the same – so it’s not too far-fetched to assume CFD-Posts Minimum/ Maximum Face Angle and ICEM’s Minimum/ Maximum Dihedral Angle are the same.

====================================

Mesh Expansion

The concept of mesh expansion relates to rate of change in the magnitude of adjacent element face areas or volumes.
The most relevant measure of mesh expansion for the CFX-Solver is illustrated below. It involves the ratio of the maximum to minimum distance between the control volume node and the control volume boundaries. Because this measure is relatively expensive to calculate for arbitrarily shaped control volumes, an alternative formulation, the ratio of maximum to minimum sector volumes, is used.



This measure and its acceptable values are tabulated below, along with a measure that is available through the CFD-Post post-processor. Values outside of the suggested acceptable range will increase sources of error that are due to the discretization of transient and body force terms.

There are 2 mesh expansion measures:
  1. Mesh Expansion Factor

    Ratio of largest to smallest sector volumes for each control volume.
    Must be less than 20.

    In ICEM I think this is called:
    • Mesh expansion factor

  2. Element Volume Ratio

    CFD-Post only. Must be less than 20.

    I don’t know if ICEM has an equivalent criterion.


====================================

Mesh Aspect Ratio

The concept of the mesh aspect ratio relates to the degree that mesh elements are stretched. The most relevant measure of aspect ratio for the CFX-Solver is illustrated below. It involves the ratio of the maximum to minimum integration point surface areas in all elements. Nodal (that is, control volume) values are calculated as the maximum of all element aspect ratios that are adjacent to the node.



The area based measure is tabulated below along with another measure that is available through the CFD-Post post-processor. Values outside of the suggested acceptable range will lead to round-off errors and associated difficulties converging the discretized equations.
  1. Aspect Ratio

    Largest ratio of maximum to minimum integration point surface areas for all elements adjacent to a node.
    Must be less than 100 for single precision solver, or less than 1000 for double precision solver.

    Not clear what this is in ICEM.

  2. Edge Length Ratio (CFD-Post)

    Same as point 1, but in CFD-Post.

    I don’t know if ICEM has an equivalent criterion.

====================================

Closing remarks:
If anyone has any input for this, or suggestions to look at any other mesh criterion for CFX then I’m all ears.
Credit to Ansys CFX Modelling guide for the pictures and literature.
Far, jbjiang, shivasluzz and 2 others like this.
JuPa is offline   Reply With Quote

Old   October 29, 2015, 03:24
Default
  #2
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
Any opinions anyone? I'm sure of this was ICEM guide for Fluent we's be on page 100 by now
JuPa is offline   Reply With Quote

Old   October 29, 2015, 20:25
Default
  #3
New Member
 
Hossam Alaa
Join Date: Nov 2014
Posts: 5
Rep Power: 7
Hossam Alaa is on a distinguished road
please, Is there any reference for these values (CFD-POST)?
Hossam Alaa is offline   Reply With Quote

Old   October 30, 2015, 03:25
Default
  #4
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
Yes, like I mentioned in the first post the reference is the CFX modelling guide. It explains what CFX requires to have a good mesh. Unfortunately the criteria CFX suggests does not match perfectly with the criteria that ICEM produces.

Both products are made by Ansys so I'm not sure why there's any disparity.
Hossam Alaa likes this.
JuPa is offline   Reply With Quote

Old   November 3, 2015, 09:22
Default
  #5
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
I've done some more investigating.

I've concluded the most reliable way to determine mesh criteria for CFX jobs are to view the mesh in CFD Post.
JuPa is offline   Reply With Quote

Old   November 3, 2015, 15:16
Default
  #6
New Member
 
Hossam Alaa
Join Date: Nov 2014
Posts: 5
Rep Power: 7
Hossam Alaa is on a distinguished road
Yes I think it is the best way to check mech quality. Even you can make one iteration only then check the mesh
Hossam Alaa is offline   Reply With Quote

Old   November 4, 2015, 04:32
Default
  #7
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
That's what I have concluded. After generating a mesh in ICEM, I load the mesh into a new CFX setup. I don't change any settings at all, except for the maximum number of iterations (1 iteration).

I then post process the results in CFD Post to determine the mesh statistics. It's a bit long winded (takes perhaps an extra 5 minutes to do) but it's the only way to be sure.

I'm not sure why there is a huge disparity between what CFX asks for and what ICEM gives you.


There should be a configuration in ICEM, like there is in Ansys Meshing where you select your desired solver (CFX or Fluent) and it provides you with the necessary details:
1. Inflation: stair step (CFX) or layer compression (Fluent).
2. Orthogonal quality of the mesh based on your solver.
3. Skewness of your mesh based on your solver.
4. Max aspect ratio and cell expansion based on your solver.
JuPa is offline   Reply With Quote

Old   November 4, 2015, 10:33
Default
  #8
New Member
 
Hossam Alaa
Join Date: Nov 2014
Posts: 5
Rep Power: 7
Hossam Alaa is on a distinguished road
I am using Ansys meshing, but how can I select my desired solver (cfx or fluent)
Hossam Alaa is offline   Reply With Quote

Old   November 5, 2015, 05:33
Default
  #9
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
Sure:



Just change Fluent to CFX.
JuPa is offline   Reply With Quote

Old   November 17, 2015, 18:13
Default
  #10
New Member
 
Przemek
Join Date: Feb 2010
Location: Warsaw Poland
Posts: 27
Rep Power: 11
Batis is on a distinguished road
Hi,

It won't add much value to the main thread but one comment from my side. To check the mesh in CFX-Post you don't need to run simulation at all. Definition file can be opened directly in post processor.
JuPa likes this.
Batis is offline   Reply With Quote

Old   November 19, 2015, 07:45
Default
  #11
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 352
Rep Power: 10
JuPa is on a distinguished road
Fantastic I didn't know that. I was running 1 iteration to get a CFX .res file and then opening up in CFD Post.
JuPa is offline   Reply With Quote

Old   September 4, 2017, 10:43
Default Difference between Orthogonality Angle Minimum and Orthogonality Angle in cfx/CFD-pos
  #12
New Member
 
chiragsvnit's Avatar
 
Chirag Trivedi
Join Date: Sep 2009
Location: Norway
Posts: 26
Rep Power: 12
chiragsvnit is on a distinguished road
Send a message via Skype™ to chiragsvnit
This is indeed useful information and thank you.
Do you know what is the difference between "Orthogonality Angle Minimum" and "Orthogonality Angle" in cfx/CFD-post?
Regards,
Chirag.
chiragsvnit is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PEM Fuel cell module meshes. ICEM vs workbench aarvay FLUENT 23 August 27, 2017 16:54
[ANSYS Meshing] Workbench 13: Structured Hexa Meshes rooftop ANSYS Meshing & Geometry 19 March 31, 2016 03:33
[ANSYS Meshing] who have the pdf of "DesignModeler User's Guide" "Meshing User's Guide" ? hotboy ANSYS Meshing & Geometry 2 August 10, 2015 22:23
Small mistake in the user's guide alberto OpenFOAM Bugs 0 February 9, 2010 21:02
ICEM CFD users centaur_ks Main CFD Forum 7 July 29, 2003 17:08


All times are GMT -4. The time now is 01:59.