CFD Online Logo CFD Online URL
Home > Forums > ANSYS Meshing & Geometry


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

LinkBack Thread Tools Display Modes
Old   March 22, 2011, 11:01
Default ICEMCFD Meshing
New Member
Sumeet Kumar
Join Date: Mar 2009
Posts: 21
Rep Power: 10
crazysumi is on a distinguished road

I am trying to mesh a geometry with hex dominant cells, Please go through the snaps I have posted here.

I have a cicular pipe on one end and a rectangular cross section box on the other end. The transition is from a circular cross-section to a rectangle. Hence there is a planar diffuser in between. I am trying to mesh this geometry using the blocking method in ICEMCFD.



Blocks with O-grid

Hex Cells - Mesh Quality - Aspect Ratio

Hex Cells - Mesh Quality - Quality

I am getting very high aspect ratio hex cells in the transition part, Can anyone assist me in having a better quality mesh. I could not figure out a way to mesh it properly in the diffuser part.

Fluent solver reports failed mesh checks:

Checking wall distance.
WARNING: The mesh contains high aspect ratio hexahedral
or polyhedral cells.
The default algorithm used to compute the wall
distance required by the turbulence models might
produce wrong results in these cells.
Please inspect the wall distance by displaying the
contours of the 'Cell Wall Distance' at the
boundaries. If you observe any irregularities we
recommend the use of an alternative algorithm to
correct the wall distance.
Please select /solve/initialize/repair-wall-distance
using the text user interface to switch to the
alternative algorithm.

P.S. : I am quite new to ICEMCFD Meshing.
crazysumi is offline   Reply With Quote

Old   March 22, 2011, 16:11
New Member
Join Date: Feb 2011
Posts: 20
Rep Power: 8
Mitpostdoc is on a distinguished road
I am quite new to Icem but I'll try to help.

It looks to me that ICEM is not correctly placing the nodes on the O-Grid internal edges. It can be more clear if you would:
right click on Pre-mesh>Scan planes
then you should swap the planes and find out what is going on inside it.

I can guess some solutions... but keep in mind that I am not an expert:
1)Extend the split on the first O-grid (the one in the round pipe) and connect it with the square section trough a more clean block structure. Check for example the one which ICEM does automatically when you create an O-Grid by selecting blocks.
2) Simply move the internal vertices around and see what happens
3) Use a different law for the nodes on the internal edges.

I hope that this was helpful.
Mitpostdoc is offline   Reply With Quote

Old   March 24, 2011, 15:40
New Member
Adrian Dunne
Join Date: Jan 2011
Location: Ireland
Posts: 26
Rep Power: 8
ad281 is on a distinguished road
you might want to try put in tetrahedral elements in that transition region.
ad281 is offline   Reply With Quote

Old   March 24, 2011, 17:46
Default Fix topology and snap to fit...
Retired from CFD Online
PSYMN's Avatar
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry, your topology is wrong and then you didn't fit your bad topology before creating your Ogrids...

Lets look at topology first...

You said it yourself, it is just a pipe with a transition... Therefore you just need a pipe type topology...

Create a single block for the length of the pipe... Associate the ends of the block to the ends of the pipe... (one end is associated to the circle, the other to the square at the opposite side...)

Then split the block twice across its length... Associate these new splits, one with the circle on the one side of the transition and the other with the rectangle on the other side of the transition...

Actually snap fit these verts into place before creating the Ogrid... The quality will already be decent except for the "corners" of the round pipe.

Then apply the ogrid... Select all three blocks for the Ogrid, also select the inlet and outlet faces... Apply.

Now your blocking is done.

Adjust your edge parameters to have the right mesh distributions, etc...
PSYMN is offline   Reply With Quote

Old   April 21, 2011, 01:22
New Member
Join Date: Jan 2011
Posts: 24
Rep Power: 8
vidhya is on a distinguished road
i too have same type of queries.. i have an inlet port in a tank through which i give my feed.. and also an outlet port. once i do hexa meshing, first i finish it for the tank region. then i went for the two ports. i have meshed it this way.. like created inidividuals blocks for the two ports and meshed it. do i have to include a block for the same in the tank cos i have the outlet attached to tank and then extruded out. so is it right that i do meshing for the ports separately and then the curved part on the tank surface separately..
i am new to this meshing thing.. please figure it out.

and also i have a bend in my inlet port which is then extruded straight for few mm.
now how do i mesh this??
vidhya is offline   Reply With Quote


Thread Tools
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 On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Question about meshing 2D airfoil in icemcfd cxcxcx0505 ANSYS 2 May 26, 2010 19:09
ANSYS ICEMCFD Streaming Meshing Demos ANSYS Main CFD Forum 2 October 22, 2004 07:55
APL/A* environment in ICEMCFD HEXA/TETRA meshing naga Main CFD Forum 0 July 23, 2004 07:06
Singularity of grid?Volume meshing vs face meshing Ken Main CFD Forum 0 September 4, 2003 11:09
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 11:08

All times are GMT -4. The time now is 05:19.