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

[ICEM] prism and convergence

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2012, 06:26
Default prism and convergence
  #1
New Member
 
Join Date: Oct 2012
Posts: 14
Rep Power: 4
Markus is on a distinguished road
Hi Everyone,


I am trying to mesh an underwater model of a satellite. I made
a prism layer around it and then a tetra mesh. The convergence is really bad in Fluent.
How do i increase the quality of the boundary layer? make especially the elements in the inner corner better?

I would appreciate any help, thank you :-)


Markus
Attached Images
File Type: jpg screen.jpg (97.5 KB, 31 views)
Markus is offline   Reply With Quote

Old   November 26, 2012, 06:35
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,104
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
What makes you so sure thar the "bad" convergence is caused by the mesh quality?
Did you evaluate some of the quality indicators?
flotus1 is offline   Reply With Quote

Old   November 26, 2012, 07:21
Default
  #3
New Member
 
Join Date: Oct 2012
Posts: 14
Rep Power: 4
Markus is on a distinguished road
Yes it seems that the quality especially in the transition between prism and tetra. and also if i have the very small prisms next to the bigger ones thats not very good right? In gambit there was this option to wedge the edges, is there something similar in icem?

Thanks, Markus


In the picture, the elements have a quality worse than 0.2
Attached Images
File Type: jpg quality.jpg (101.7 KB, 25 views)
Markus is offline   Reply With Quote

Old   November 26, 2012, 07:31
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Hey I gave you the fully hexa mesh!!! did you try it? Boundary layer direction
Far is offline   Reply With Quote

Old   November 26, 2012, 07:34
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
for prisms quality of 0.01 is good enough for fluent.
Far is offline   Reply With Quote

Old   November 26, 2012, 07:35
Default
  #6
New Member
 
Join Date: Oct 2012
Posts: 14
Rep Power: 4
Markus is on a distinguished road
hey

Yes but i didnt manage to make the mesh. It never created the volumes, only surface mesh.
Markus is offline   Reply With Quote

Old   November 26, 2012, 07:36
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Right click on premesh and then select convert to unstructured mesh. Afterwards follow the same procedure you followed for the prsim+tetra mesh i.e. boundary conditions, selection of solver and then output.
Far is offline   Reply With Quote

Old   November 26, 2012, 10:03
Default
  #8
New Member
 
Join Date: Oct 2012
Posts: 14
Rep Power: 4
Markus is on a distinguished road
Ok thanks..
I ran it with fluent but the result can not be right.

I put the laminar solver
Attached Images
File Type: jpg residuals.jpg (53.5 KB, 16 views)
Markus is offline   Reply With Quote

Old   November 26, 2012, 10:06
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Why laminar? Whats the Reynolds Number? May be your problem is transient!!!

can you attach your case file?
Far is offline   Reply With Quote

Old   November 26, 2012, 11:35
Default
  #10
New Member
 
Join Date: Oct 2012
Posts: 14
Rep Power: 4
Markus is on a distinguished road
Reynolds number is around 60000

0.2 m/s flow

I thought as long as it doesnt work with the laminar model it wont with the turbulent either..

ill send you the case file per mail
Markus is offline   Reply With Quote

Old   November 26, 2012, 12:26
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Few things

1. Boundary conditions

I would prefer to define the upper, lower, right side and left side faces as wall with slip condition instead of pressure outlet.

2. Domain

Increase the domain size : Inlet at 15*L and outlet at 25*L

3. Mesh
Most important factor
The hexa mesh is still not finalized model, you need to set the edge mesh parameters, sizing, expansion rate, edge mesh matching, y+ consideration if turbulence is importnat (ever in case of laminar model you need to resolve the shear layers so make sure that the mesh is refined in important areas) etc to make it pleasant to solver.

4. Solver
Try pressure based coupled solver.


5. Flow scheme
First start with 1st order convection scheme then switch to 2nd order.

6. Turbulence or laminar
Also try turbulence model along with transition model.

PS: I believe there would be high level vortex shedding behind your object due to many protruded bodies.
Attached Images
File Type: jpg satellite1.jpg (52.5 KB, 16 views)
File Type: jpg satellite2.jpg (93.9 KB, 13 views)

Last edited by Far; November 26, 2012 at 12:51. Reason: Images
Far is offline   Reply With Quote

Old   November 27, 2012, 11:52
Default
  #12
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,104
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Please use some kind of turbulence modeling for turbulent flows. If it still does not converge, you can still spend some time on improving the mesh.
Simulating a turbulent flow as an underresolved DNS cannot create correct results.
flotus1 is offline   Reply With Quote

Old   November 28, 2012, 10:48
Thumbs up
  #13
New Member
 
RZA
Join Date: Nov 2012
Posts: 25
Rep Power: 4
Engr.RZA is on a distinguished road
I think the you should try the last steps as mentioned by FAR.

Your Reynolds number suggest that you can assume laminar flow.

Regards,

RZA
Engr.RZA is offline   Reply With Quote

Reply

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
Convergence and discretization karananand FLUENT 3 August 29, 2010 06:07
Discretization and convergence karananand Main CFD Forum 0 August 4, 2010 16:19
early stall, poor convergence, and mesh quality everest CFX 2 May 12, 2010 16:27
Convergence issue in SST for Porous model Raj CFX 0 May 2, 2008 02:43
problem in convergence with the prism layer genera rakesh CFX 3 September 18, 2006 10:13


All times are GMT -4. The time now is 10:21.