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

[ICEM] Smooth Transition for Tet Prism meshing

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2013, 11:07
Default 3D meshing with prism layers on wall boundaries
  #21
New Member
 
katerina
Join Date: Feb 2013
Posts: 5
Rep Power: 5
katarin is on a distinguished road
Quote:
Originally Posted by saisanthoshm88 View Post
In Ansys WorkBench, I find the option "smooth transition" very useful for generating Inflation / Prism layers as it helps in maintaing a good volume transition between the last layer prisms and the tetras.

Could some one please let me know if there is a analogus option for prism meshing in ICEM CFD.
Hello,

I am new in ANSYS CFX. I want to solve a Dam Break problem with rectangular volumes. I have designed the 2 volumes in CATIA, and want to make a mesh with the CFD mesher. I need the 2 big cross sides to have an unstructured mesh, and make 100 laylers of it, through it' s height.

I have tried it with inflation, which seems the only way to do it, but it gives me a structured mesh.
Could somebody help me?

Thanks in advance
katarin is offline   Reply With Quote

Old   February 22, 2013, 11:10
Default
  #22
New Member
 
katerina
Join Date: Feb 2013
Posts: 5
Rep Power: 5
katarin is on a distinguished road
Quote:
Originally Posted by katarin View Post
Hello,

I am new in ANSYS CFX. I want to solve a Dam Break problem with rectangular volumes. I have designed the 2 volumes in CATIA, and want to make a mesh with the CFD mesher. I need the 2 big cross sides to have an unstructured mesh, and make 100 laylers of it, through it' s height.

I have tried it with inflation, which seems the only way to do it, but it gives me a structured mesh.
Could somebody help me?

Thanks in advance
I forgot to mention that i need to make wedge prisms.
Thank you
katarin is offline   Reply With Quote

Old   March 19, 2016, 10:30
Question
  #23
New Member
 
Suyash Sharma
Join Date: Feb 2016
Posts: 7
Rep Power: 2
Quasar_89 is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Sure... The tech actually comes from ICEM CFD first

In ICEM CFD global prism settings, you can set 3 of the 4 prism settings. You can set initial height, number of layers, ratio and/or total height. Setting three gives enough to calculate the 4th.

However, if you leave initial height and total height as 0, a nonsensical number, you have left Prism with enough freedom to float the initial height based on the first cell size. The initial height is adjusted at each column, with respect to the number of layers and ratio, to result in a last prism height that is similar in volume to its adjacent tetra...

If you use this, you actually need to put in the number of layers and ratio that you want. You can't pull the "1 layer and split" trick.

In older version (I think before R13 or so), if you set the initial height on any part or entity, it would stop this from working. But more recent versions are more flexible and allow you to have a global float and specific heights on only certain parts or surfaces.

Dear Simon,

I have been looking at your posts on Tet/Prism and other documents by you for the case and i have been able to achieve a very high quality mesh (min 0.3+ and mean quality 0.8+ ). Where i struggle is when the volume is Robust Octree, i get about 4 million cells but applying delaunay reduces element count to 1.7 million from there. Now for my application (Ahmed Body in wind tunnel, following Lienhart et. al experimental setup ) i need coarse, medium & fine mesh as 0-5 , 5-10 & 10+ respectively following Y+ s of 300, 150 & 50 respectively. I have been able to split my prisms and redistribute but even then i am not able to achieve anything higher than 2.5 million for obvious reasons.

Can you guide me in how to achieve my desired element count? I tried global cell refinement but it looked really artificial and inappropriate. I am stuck with this and there seems to be absolutely no discussion on element count anywhere when doing Tet/Prism meshing.
Quasar_89 is offline   Reply With Quote

Old   March 19, 2016, 12:21
Default
  #24
Member
 
Lorenzo Mazzei
Join Date: Dec 2010
Posts: 38
Rep Power: 7
Mazze[ITA] is on a distinguished road
Quote:
Originally Posted by Quasar_89 View Post
Dear Simon,

I have been looking at your posts on Tet/Prism and other documents by you for the case and i have been able to achieve a very high quality mesh (min 0.3+ and mean quality 0.8+ ). Where i struggle is when the volume is Robust Octree, i get about 4 million cells but applying delaunay reduces element count to 1.7 million from there. Now for my application (Ahmed Body in wind tunnel, following Lienhart et. al experimental setup ) i need coarse, medium & fine mesh as 0-5 , 5-10 & 10+ respectively following Y+ s of 300, 150 & 50 respectively. I have been able to split my prisms and redistribute but even then i am not able to achieve anything higher than 2.5 million for obvious reasons.

Can you guide me in how to achieve my desired element count? I tried global cell refinement but it looked really artificial and inappropriate. I am stuck with this and there seems to be absolutely no discussion on element count anywhere when doing Tet/Prism meshing.

You could reduce the global scale factor and apply local density to refine the areas of interest.
Mazze[ITA] is offline   Reply With Quote

Old   March 19, 2016, 12:57
Default
  #25
New Member
 
Suyash Sharma
Join Date: Feb 2016
Posts: 7
Rep Power: 2
Quasar_89 is on a distinguished road
Hello Mazze,

I am sorry to have not mentioned it before, but i did think of using a <1 scale factor to multiply cell count but just didn't apply yet in between my other attempts such as global refinement number as 18 and min. size limit of 0.006 since my topology tolerance was 0.05.

The problem with using sclae factor is that i want to use certain sizes for my mesh and if i change my scale factor i will need to change my cell sizes accordingly.
For example i want a max cell size of 150 , and for the ahmed body itseld, i want a max cell size of 10mm , which is restricted as per the best practices guide for a given Y+ & velocity inlet speed.

What i can see here is there is no way out from it unless cell sizes be refined by one or the other way and in every way out, the max cell size is reduced either by direct refinement or by using a scale factor less than 1.
So i'm going to try and pull off my restriction on max cell size and see what do i get out of this.

And i am already using a density region in the wake of the ahmed body.

Thanks for a quick response though.
Quasar_89 is offline   Reply With Quote

Old   March 19, 2016, 15:30
Default
  #26
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 184
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
Are you using symmetry? I mean, the fastest way to increase your element count is to stop using symmetry
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   March 19, 2016, 16:06
Default
  #27
New Member
 
Suyash Sharma
Join Date: Feb 2016
Posts: 7
Rep Power: 2
Quasar_89 is on a distinguished road
Hi Alex,

I'm using symmetry just as you did in your youtube tuts and everybody else did in this computational experiments as well. Some researchers like hinterberger have been able to reach very high values of element count using same domain size as lienhart et. al 2000, applying symmetry. So howcome i'm nowhere even close to that. I did reach 4 million with octree but delaunay just delineated my whole progress... and put me down on 1.7 million approx.
And it's as if i'm the only one who's facing this problem or have faced this problem.

PS : My classmate is having a good time following your tutorial on ahmed body step to step.
Quasar_89 is offline   Reply With Quote

Old   March 19, 2016, 16:33
Default
  #28
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 184
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
If you're using the document "Best practice guidelines for handling Automotive External Aerodynamics with FLUENT" from German Fluent guys (that I linked below the videos, I think), then I know where your problem is (most likely).

What they were suggesting was to use first-aspect-ratio method to grow prisms. So, let's say for example you had 20 mm triangles all over the body and you grow 5 prisms out of that using the F-A-R of 5 and growth rate of 1.2. This should result in an average y+~300 and you have your "coarse mesh".

Then, the only way to reduce y+ for the medium mesh (F-A-R of 5 remains) is to have 10 mm triangles all over the body. This would give a mesh with y+~150.

If you wanted a y+~50 mesh next, this means dividing the previous surface element by 3, so now you'd cover the whole body with 3 mm surface elements. As you can see, the mesh size would grow very rapidly.

Another problem you have in ICEM CFD is that you're creating your initial surface mesh using Octree and you will never have any control over the surface mesh growth ratio because octree can only use a "power of 2" during refinements (proximity or curvature) and then with subsequent normal or Laplace smoothing you can get it to look as if it's growing smoothly. But if you "zoom out" far enough, it's always growing in "power of 2" steps (2 mm, 4 mm, 8 mm, 16 mm etc.) and you can't really create anything in between. You can cheat with scaling factor for the entire mesh, but that doesn't really solve your problem.

What I'd recommend is go back to ANSYS Meshing and create meshes with different volume growth rates. So, use max 10 mm body surface elements (maybe even 2 mm for the legs/stilts) but set the overall mesh growth rate to 1.2 in the first case, then 1.15, then 1.10 and you'll see how fast your cell count grows. Also, switch the meshing algorithm to advancing-front instead of the regular one. This will give you a very smoothly growing surface and volume mesh.

I'm guessing you're still using just prism + tetra meshes? This method should be able to grow element counts without problems. I know when I moved on to hex tunnel or hexacore meshes I could usually get the same flow resolution with just half the elements or less. Last time I attempted this I think the symmetric Ahmed body case was captured with y+~70 on the straight surfaces of the body (and around 100 on the front curved faces) with just 800 000 cells in the mesh. I didn't even do a grid independence study because the results with this approach were already beyond reproach.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy 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
[ANSYS Meshing] Prism meshing mahesh_1402 ANSYS Meshing & Geometry 0 January 30, 2012 01:10
ICEM Prism Layer transition between surface with prism layers and one without TWaung ANSYS Meshing & Geometry 2 October 12, 2009 14:56
prism meshing??? Nitin Dewangan CFX 1 August 1, 2008 18:35
ICEM - problems with prism mesh João Lourenço CFX 1 November 6, 2007 15:41
ICEM 10 smooth transition error Stephen CFX 3 March 13, 2007 10:23


All times are GMT -4. The time now is 16:24.