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

boundary layer in gambit

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2013, 09:40
Default boundary layer in gambit
  #1
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
dear all,
I want to add a boundary layer to this kind of shape, but as much as I tried, I still couldn't get it right.
These two pics shows a mesh I created lately, obviously the boundary layer is in bad shape at the corners.
How can I get a boundary layer closely resembles the geometry?
Attached Images
File Type: jpg 1.JPG (23.1 KB, 17 views)
File Type: jpg 2.JPG (44.4 KB, 19 views)
kkpal is offline   Reply With Quote

Old   October 1, 2013, 00:43
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
by clicking right mouse (or midlle ?) you can switch the orientation.
But the question is: why do you have fluid cells on both sides of your wall edge?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 1, 2013, 01:24
Default
  #3
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
hi max,
no, I dont have fluid cells on both sides, it's just on the outside wall.
I'm simulating flow around this kind of cylinder, later this shape will be extruded into 3D.
It seems right or middle clicking did not change the orientation of the boundary.Can you elaborate more about that?

Quote:
Originally Posted by -mAx- View Post
by clicking right mouse (or midlle ?) you can switch the orientation.
But the question is: why do you have fluid cells on both sides of your wall edge?
kkpal is offline   Reply With Quote

Old   October 1, 2013, 01:53
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
if the bl is pointing in this direction, it means the bl can grow in this direction.
Then you have a surface, in which the bl can be applied.
Enable shaded mode, you will see if you have a surface.
I confirmed the middle mouse click for switching BL direction. But it will switch only if it can (understand if you have a surface on the other side)
Untitled1.png Untitled2.png
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 1, 2013, 03:03
Default
  #5
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
hi,max
In my case, I'm meshing the outside boundary of the shape, however, at the corner, the mesh quality seems very bad and I want to modify it.
I think what you mean is changing the boundary layer to the inside of the wall.. that's not quite exactly what I wanted.
Lately I find out that when the boundary layer is thin, the mesh is in good condition. While the layer grows thicker, the mesh at the corner becomes skewed. Here I post two pics for illustration. The first one is thick bl, and the second one is thin bl.


Quote:
Originally Posted by -mAx- View Post
if the bl is pointing in this direction, it means the bl can grow in this direction.
Then you have a surface, in which the bl can be applied.
Enable shaded mode, you will see if you have a surface.
I confirmed the middle mouse click for switching BL direction. But it will switch only if it can (understand if you have a surface on the other side)
Attachment 25717 Attachment 25718
Attached Images
File Type: jpg 1.JPG (82.9 KB, 10 views)
File Type: jpg 2.JPG (37.5 KB, 7 views)
kkpal is offline   Reply With Quote

Old   October 1, 2013, 03:13
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
Quote:
Originally Posted by kkpal View Post
that's not quite exactly what I wanted..
ok I missunderstood, sorry.
Then the problem comes from the depth of your BL.
If your y+ enables you try to reduce first row height, and increase number of layer
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 1, 2013, 03:53
Default
  #7
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
ok I missunderstood, sorry.
Then the problem comes from the depth of your BL.
If your y+ enables youm try to reduce first row height, and increase number of layer
yeah ,that seems the only way to get it right. I was hoping there is a way to create mesh like this.
thanks for your kind help!
Attached Images
File Type: jpg 3.JPG (39.3 KB, 13 views)
kkpal is offline   Reply With Quote

Old   October 1, 2013, 03:58
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
sure you can, but on the picture the red mesh isn't a BL
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 2, 2013, 00:28
Default
  #9
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
sure you can, but on the picture the red mesh isn't a BL
Your words really gave me hope!
In another thread(Gambit mesh for cylinder ) you told me to do some split on the cylinder surface, I will try that.
And if my attempt fails, I will ask you for help.
Thanks!
kkpal is offline   Reply With Quote

Old   October 2, 2013, 03:13
Default need help!!
  #10
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
hi, max.
My attempt failed. I don't even have a clue where to do the splits
Given the geometry of cylinder with helix, can you tell me how to generate that kind of beautiful mesh in gambit?
Here is a similar thread I posted some days ago.
From Autocad to Gambit, what is the mesh strategy?
kkpal is offline   Reply With Quote

Old   October 2, 2013, 09:42
Default
  #11
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 920
Rep Power: 15
ghost82 will become famous soon enough
If the boundary layer failed, you can try to add some extra surface and make "your boundary layer" in these surfaces, by manually create the mesh as the boundary..this is just a suggestion..

Daniele
ghost82 is offline   Reply With Quote

Old   October 3, 2013, 01:48
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
Quote:
Originally Posted by kkpal View Post
hi, max.
My attempt failed. I don't even have a clue where to do the splits
Given the geometry of cylinder with helix, can you tell me how to generate that kind of beautiful mesh in gambit?
Here is a similar thread I posted some days ago.
From Autocad to Gambit, what is the mesh strategy?
For having similar mesh as in your picture you need do split your domain with a straight cylinder which will surroung your helicoid.
Then in this new domain, apply a BL on helicoidal walls and apply also a size fonction)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 4, 2013, 04:12
Default
  #13
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
hi max,
Inspired by your suggestion, I successfully created good mesh around the helixcoid. Here is my procedure.
1. mesh the top and bottom edges; 2. mesh the helixcoid face with quad/submap, it automatically generated good quad mesh on the cylinder surface; 3. apply bl on the cylinder surface; 4. mesh the domain.
However, in the second step, it seems difficult to control the axial mesh size. Usually the mesh in the axial direction is too dense for my simulation.
Is there a way to solve this problem? I realize there is a SPACING column, I changed the value in it but result did not change.
And is there a way to view the mesh inside the domain? like the third picture.
Attached Images
File Type: jpg 1.JPG (41.1 KB, 9 views)
File Type: jpg 2.jpg (102.7 KB, 8 views)
File Type: jpg 3.JPG (35.8 KB, 10 views)
kkpal is offline   Reply With Quote

Old   October 4, 2013, 04:21
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
from your first picture I don't see any split as I adviced you.
Create a cylinder with radius greater than your helicoid, then split your domain with the cylinder volume.
At the end you should have 2 volumes: the one next to your helicoid and the rest
Doing that you will have more control on your mesh
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 4, 2013, 05:02
Default
  #15
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
and one more strange thing.
in the face mesh, sometimes the Proj Interval column appears, but most of the times it does not.
I believe that option can control the axial mesh size.
How can i make it appear?
kkpal is offline   Reply With Quote

Old   October 4, 2013, 05:17
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
It appears only with quad
https://www.sharcnet.ca/Software/Gam...proj_intervals
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 4, 2013, 05:36
Default
  #17
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
thanks max,
I created a circular cylinder surround the helixcoid, and meshed the circular cylinder surface with approiate axial mesh size by specifying Proj interval . Then I mesh the domain with Hex, I suppose by doing this the axial mesh size on the helixcoid would be the same with the outer cylinder, but after two trial it didn't, the mesh on the helixcoid is still not controllable.
what is the way to control that?
and btw is there a button in gambit for view the mesh in side volume?
Attached Images
File Type: jpg 8.JPG (49.4 KB, 3 views)
File Type: jpg 7.jpg (101.3 KB, 10 views)
kkpal is offline   Reply With Quote

Old   October 4, 2013, 06:15
Default
  #18
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
mesh helixcoid surface first, then create a size function with helixcoid surface as source and top (or bottom) cap from cylinder as attachment.
Give the desired parameter mesh expansion.
Mesh the cap surface.
Now you have one cap and also the axial direction which are meshed.
You can go and mesh the volume with cooper. Gambit should select automatically the source for cooper.
for your last question, go to examine mesh, and work with plane
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 5, 2013, 12:04
Default
  #19
Member
 
Kai
Join Date: Jan 2013
Location: Japan
Posts: 89
Rep Power: 4
kkpal is on a distinguished road
hi max,
I tried meshing the helixcoid surface first, but for this 10m-high helixcoid Gambit automatically generated 566 nodes in the axial direction. And with 180 nodes along the Circumference, the helixcoid surface alone owns 101880 nodes! And when I use Cooper to perform volume mesh, my machine went break!
Now I'm thinking using the journal file to enforce a Proj interval on my helixcoid surface, since this option did not appear even though I chose Quad to do the meshing.
But is there another way to reduce the axial mesh quantity in the axial direction of the helixcoid?
kkpal is offline   Reply With Quote

Old   October 9, 2013, 00:41
Default
  #20
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
Axial node distribution can be reduced, it will only influence the aspect ratio of your cells (hexa or wedge)
You can dramatically reduce mesh size by playing with size function's parameters.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- 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
Low Mixing time Problem Mavier CFX 5 April 29, 2013 00:00
Probems in Gambit: trouble linking two faces when a boundary layer is applied Kathryn39 ANSYS Meshing & Geometry 1 August 8, 2012 13:11
Questions about Boundary Layer Thickness and Turbulence Models famerfamer STAR-CCM+ 3 July 12, 2012 09:47
Gambit boundary layer pixie Main CFD Forum 1 September 30, 2009 12:22
GAMBIT problem with 3D Boundary Layer when meshing Anthony Haroutunian FLUENT 2 March 26, 2008 03:02


All times are GMT -4. The time now is 13:32.