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

[ICEM] Some meshing quieries with ICEM CFD

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 6, 2011, 07:09
Default Some meshing quieries with ICEM CFD
  #1
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Is it advantageous to grow prisms from a surface mesh and then fill the volume with tetras by some bottom up approaches like Delaunay?

What is the advantage of setting a different height on each curve on the opposite sides of the prism surface?

How do structured mesh solvers function, do they require the blocks along with the mesh to locate the nodes?

I’ve loaded a massive CAD model (STEP file) in ICEM CFD and I couldn’t freely perform operations like – Rotate, zoom (or) pan then I’ve increased the number of processors used to 3 by going to SettingsąGeneral and tried even by setting the Max Display List Size to 1000 MB but these didn’t show any effect and the difficulty still persisted.

What is the acceptable range of quality for pyramid elements to solve in CFX?

Can some one please suggest me upon these issues?
__________________
Best regards,
Santhosh.

Last edited by saisanthoshm88; April 6, 2011 at 10:17.
saisanthoshm88 is offline   Reply With Quote

Old   April 6, 2011, 14:50
Default Prism Questions
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Wow, each of these could probably get its own thread. I have a moment while my CPU is chugging and will just look after the prism issues here.

1) Yes, many users (including myself) start with OCTREE to get the patch independent surface mesh, then delete the volume mesh, smooth the heck out of the surface mesh (with alternating iterations of laplace on then laplace off), grow a new Delaunay mesh and then insert prism... Others switch the last two steps and grow the prism first and then fill with delaunay tetra; this is faster because prism doesn't need to move the tetras out of the way, but the danger there is that prism can't use the tetras to avoid penetration across a gap (prism is not as smart without the tetras). There is a third option of growing prisms into a tetra mesh (either the original octree or the delaunay) and then deleting the tetras and growing new tetras with delaunay (post prism), this prevents any problems with using prism stand alone and could generate a nicer transitioning mesh in some cases, but often the faces on the inside of the prism layer are lower quality than the triangles at the surface and it is possible that tetra will fail... I always keep the inserted tetra layer as a backup...

2) If you set a different height on the curves on either side of a tetra surface, the prism height will transition across the surface. But you must be careful not to set a height on the surface its self or it will over ride the transition.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 8, 2011, 11:48
Default
  #3
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Thanks for the replies Simon. Please answer the other questions when ever you find some time.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   April 18, 2011, 15:03
Default
  #4
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Hi Simon,

After a bit of exploration in the net I was able to locate some info. on structured solvers , that can answer my question-

" The "blocks" in a multi-block mesh are simply the "sub-grids" that are
used to fill up the computational domain. In that sense, a structured
multi-block grid can be thought of as a coarse unstructured mesh where
each unstructured cell is itself a structured grid.

The advantage of structured solvers (when you can create a good
structured grid) is that that they are typically much faster (on a time
per point per iteration basis). The difference can be an order of
magnitude or more. This is due to the way that the properties at a
point and its neighbors can be accessed very efficiently. It is much
faster for the computer to find q(i,j+1,k,1) than to look up
rho(neighbor(mycell)%cell(ngbr)). Indirect memory addressing carries a
pretty big performance penalty."


Regarding the pyramid quality issue I found that something > 0.05 or 0.1 is fine and acceptable

Can you please answer the question on the memory settings in ICEM CFD -

I’ve loaded a massive CAD model (STEP file) in ICEM CFD and I couldn’t freely perform operations like – Rotate, zoom (or) pan then I’ve increased the number of processors used to 3 by going to SettingsąGeneral and tried even by setting the Max Display List Size to 1000 MB but these didn’t show any effect and the difficulty still persisted.

__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   April 18, 2011, 16:40
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I am not an expert on hardware, etc. but I can tell you that rotating a large model is more a function of your graphics processor than your number of CPUs. There may also be a ram component, since the model is all up in memory at once, but mostly, it is your graphics card that determines the speed.

There are display settings for open GL, etc. You could play with those. I really am no expert in this area.

Simon
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 19, 2011, 07:42
Default
  #6
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Thanks for the reply Simon. Ill try to explore upon this. By the way can you please try to organize more webinars of ICEM CFD
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   April 19, 2011, 12:55
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
On what topic would you like to see ICEM CFD Webinars?
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 19, 2011, 13:21
Default
  #8
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
Simon, if your making tutorials for the ANSYS youtube site. Please can you make an ANSYS Meshing Application one showing how to mesh a vehicle (car, train, aircraft etc) inside a fluid domian for a viscous external aerodynamics CFX simulation?

I'm finding that the Meshing Application is a real pain compared to ICEM and CFX-Mesh (may it rest in peace) in so far as accessing/setting-up the vehicle mesh inside the fluid domain. Or if you have some already could you point me in the right direction to see them?

Thanks.
siw is offline   Reply With Quote

Old   April 21, 2011, 11:49
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
SIW, Hexa or Tetra/Prism?

Also, if you can email me with more specifics about what you miss from CFXMesh, I can pass it to the ANSYS Meshing product manager for his consideration.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 22, 2011, 04:42
Default
  #10
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
Simon, I would like to see a tetra/prism mesh in ANSYS Meshing Application (lets call it AMA for simplicity) since the "true" ICEM type multi-block structured meshing ability is not in AMA (yet?).

Lets take as an example a cubiod domain (1 inlet face, 1 outlet face & 4 farfield faces) with a vehicle within the centre of this cuboid. In CFX-Mesh it was very easy specify these 6 faces as Composite 2D Regions, then hide them which would allow me get access to and assign Composite 2D Regions to the whole or individual/collective faces of the vehicle (e.g. the entire aircraft or separalety for wings/fuselage etc). I understand that to reapeat this in AMA I would use Named Selections in the same way, but I find the selcting/unselecting of faces not as simple as in CFX-Mesh.

Another feature of AMA is "scoping". What is it & why is this needed? Surely, we just need to pick a cuvre/face/body and set a sizing to it.

But the most significant part of CFX-Mesh that has not been carried over, for me, to AMA is the Point/Line/Triangle Controls. I know that there is the Body of Influence. But I just don't think that geometrical entities should be assigned during the CAD process (pre-meshing process) for using for mesh sizing (I always used them for mesh sizings in wakes). This was so easy in CFX-Mesh to set-up, preview a mesh. Then if it needed to be changed then I could easily do that in CFX-Mesh - not have to get out of AMA and go into DesginModeler to make the change - BTW I don't ever use DM since Solid Edge is our CAD package of choice.

Okay this bit was never a GUI feature in CFX-Mesh but since I prefere to use ICEM I've become used to it. What does AMA do about checking & smoothing? There's no GUI options that I can see for it. Maybe it'll be there at v14.

So one of your youtube videos for AMA on an external viscous aero domain would be really helpful.

Thanks
siw is offline   Reply With Quote

Old   April 22, 2011, 07:05
Default
  #11
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Simon , I'd like to see a webinar on ICEM Hex meshing
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   April 22, 2011, 12:19
Default
  #12
Member
 
Join Date: Mar 2011
Location: Canada
Posts: 35
Rep Power: 6
Jeremie84 is on a distinguished road
Hello,
It is not the first time that I read this idea for the surface mesh of "alternating iterations of laplace on then laplace off". I am just wondering : do you recommend to end with laplace on or off ? I'd say off but it's just to be sure.

Also, for smoothing the volume mesh, each time I am wondering if I have to smooth both the tri and tetra elements, or if I have to smooth the tetras with the tri elements frozen. In other words, when I smooth both the tris and the tretas, do I "spoil" the initial surface mesh smooth ?
For the volume mesh smooth, I am not using the Laplace smoothing. Is that correct ?

Thank you for your help and your useful posts.

Jeremie
Jeremie84 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
Learn ANSYS ICEM CFD easy_astronaut ANSYS 2 December 15, 2013 16:34
icem cfd ai environment 11.0, laptop keyboard problem, linux pertupd Hardware 3 October 3, 2011 08:27
[ICEM] Export unstructured periodic mesh from ICEM CFD to Fluent ivanddd ANSYS Meshing & Geometry 1 February 3, 2011 01:51
ICEM CFD Modules Boris FLUENT 1 March 12, 2004 15:37
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 10:32.