# [ANSYS Meshing] Very high aspect ratio

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 15, 2011, 03:53 Very high aspect ratio #1 New Member   zhao xin Join Date: Feb 2010 Location: Goteborg Posts: 28 Rep Power: 9 Sponsored Links Hi, I used Ansys meshing to create a mesh with 10E-6 m first boundary layer height. There are few elements with crazy aspect ratio, around 2000000.....What can I do with this? and unbelieveable I did't get any warning. I used this mesh to run the simulation with double precision and no divergence happened, the result oscillated because of large seperation of the flow. Can i trust this? What can happen with such high aspect ratio? Thank you Kind Regards,

 August 16, 2011, 04:14 #2 New Member   Zhang Yang Join Date: Jun 2011 Location: Zürich Posts: 28 Rep Power: 9 10^-6 m thickness of first Bundary layer? What do you simulate actually? Let's say the number of Prism Layer is usually between 10 - 15 and the total height of BL depends on the flow behaviour and your expectation. But usually is between cm and m. Check the physics and think about whether you really need such tiny thin BL. In your case, if the thickness is 10^-6 (Height )and cell size (Length) is in cm, of course you will get a cray aspect ratio.

August 16, 2011, 05:26
#3
New Member

zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by swiss_zhang 10^-6 m thickness of first Bundary layer? What do you simulate actually? Let's say the number of Prism Layer is usually between 10 - 15 and the total height of BL depends on the flow behaviour and your expectation. But usually is between cm and m. Check the physics and think about whether you really need such tiny thin BL. In your case, if the thickness is 10^-6 (Height )and cell size (Length) is in cm, of course you will get a cray aspect ratio.
Thanks for the reply.
I do need the 10e-6 thickness to get y+ around 1, since I have really high pressure and mach number. Actually I am using mm as the cell size, but there is still some crazy elements. I could not get even smaller cell size due to the enormous number of elements already.

And I have 30 layers to get a relative smooth transition from the BL to the normal flow.

 August 16, 2011, 05:49 #4 New Member   Zhang Yang Join Date: Jun 2011 Location: Zürich Posts: 28 Rep Power: 9 Do you simulate supersonic flow?

August 16, 2011, 06:17
#5
New Member

zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by swiss_zhang Do you simulate supersonic flow?
No, but the Re is 10^6 with high temperature, small ref.length and high pressure. I used Grid spacing calculator http://geolab.larc.nasa.gov/APPS/YPlus/, to calculate my first layer height. And I also calculate the y+ in the result. I'm sure i need 10e-6.

 August 16, 2011, 06:25 #6 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 268 Rep Power: 19 Can you just use wall functions? Stu Last edited by stuart23; August 16, 2011 at 06:51.

August 16, 2011, 08:55
#7
New Member

Zhang Yang
Join Date: Jun 2011
Location: Zürich
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by stuart23 Can you just use wall functions? Stu
Absolutely right, Why don't you use the wall function?

Instead of creating a very fine mesh in BL, you can use the wall function. Because the Velocity Profile in BL is predictable and therefore is approximated using Wall Function. Since you want to capture more details in the BL, you can use the SST Turbulence Model and Automatic Wall Function.

Last edited by swiss_zhang; August 16, 2011 at 09:16.

 August 16, 2011, 09:13 #8 New Member   Zhang Yang Join Date: Jun 2011 Location: Zürich Posts: 28 Rep Power: 9 Actually there are 2 methods to solve the flow behaviour near the wall: 1: Wall Funtion Methode For wall function: y+ < 300 is ok delta_y = L*y+ * (74)^2*Re^(-13/14), using this formular to estimate the first node spacing delta_y, if the flow passes over a plate 2: Low-Reynold-Number Methode For Low-Reynold-Number Methode: y+ < 2

 August 16, 2011, 09:17 #9 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 Also, aspect ratio isn't everything... You can still have a high aspect ratio (though yours is very very high) and have a happy solver if your angles, skewness, etc. are all still good. This is usually fine with boundary elements... __________________ ----------------------------------------- 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

 August 16, 2011, 09:23 #10 Senior Member   Stuart Buckingham Join Date: May 2010 Location: United Kingdom Posts: 268 Rep Power: 19 Slightly off topic, but can someone advise if multigridding speed up the rate of convergence for very fine prism layers? Because the layer is so thin, the velocity gradient normal to the surface would be very small between cells (i.e. low frequency), and therefore would take a lot of iterations without multigridding. I was just wondering out of curiosity...

August 16, 2011, 09:43
#11
New Member

zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by stuart23 Can you just use wall functions? Stu
Yes, I have tried that. Maybe I should stick on the wall function.

August 16, 2011, 09:46
#12
New Member

zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by swiss_zhang Absolutely right, Why don't you use the wall function? Instead of creating a very fine mesh in BL, you can use the wall function. Because the Velocity Profile in BL is predictable and therefore is approximated using Wall Function. Since you want to capture more details in the BL, you can use the SST Turbulence Model and Automatic Wall Function.
Thanks for your effort. I was too aggressive to get the accurate BL. I will estimate them both.

August 16, 2011, 09:49
#13
New Member

zhao xin
Join Date: Feb 2010
Location: Goteborg
Posts: 28
Rep Power: 9
Quote:
 Originally Posted by PSYMN Also, aspect ratio isn't everything... You can still have a high aspect ratio (though yours is very very high) and have a happy solver if your angles, skewness, etc. are all still good. This is usually fine with boundary elements...
It's really high....yeah...but the most amazing thing is i didn't get any warning and it ran very well. Mybe it's not that critical at the boundary.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [GAMBIT] High aspect ratio RGRUIZ ANSYS Meshing & Geometry 17 September 21, 2010 02:24 Flavio CFX 2 November 24, 2006 13:01 matthias CFX 3 October 20, 2006 02:55 Andrea CFX 2 October 11, 2004 05:12 zago FLUENT 0 May 19, 2004 02:37