CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Some meshing quieries with ICEM CFD (

saisanthoshm88 April 6, 2011 07:09

Some meshing quieries with ICEM CFD
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?

PSYMN April 6, 2011 14:50

Prism Questions
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.

saisanthoshm88 April 8, 2011 11:48

Thanks for the replies Simon. Please answer the other questions when ever you find some time.

saisanthoshm88 April 18, 2011 15:03

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.

PSYMN April 18, 2011 16:40

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.


saisanthoshm88 April 19, 2011 07:42

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

PSYMN April 19, 2011 12:55

On what topic would you like to see ICEM CFD Webinars?

siw April 19, 2011 13:21

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?


PSYMN April 21, 2011 11:49

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.

siw April 22, 2011 04:42

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.


saisanthoshm88 April 22, 2011 07:05

Simon , I'd like to see a webinar on ICEM Hex meshing

Jeremie84 April 22, 2011 12:19

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.


All times are GMT -4. The time now is 08:57.