CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > Pointwise & Gridgen

How to eliminate the skewed elements when using T-REX on a wing

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

Like Tree6Likes
  • 1 Post By rmatus
  • 1 Post By rmatus
  • 1 Post By rmatus
  • 1 Post By rmatus
  • 1 Post By rmatus
  • 1 Post By rmatus

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 21, 2017, 08:30
Default How to eliminate the skewed elements when using T-REX on a wing
  #1
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Hi,

Attached are some pictures of a wing i am trying to mesh, however I get highly skewed elements around the sharp trailing edge and the leading edge, in addition the prism layer seems too large.

I used the setting in shown in the picture , I tried to play with the maximum angle criteria and Equi-angle , but always the same problem.
I defined the wing as a wall boundary condtions with a DeltaS of 1e-5.

It is worth mentioning that I would like to have a tetrahedral region around the trailing edge tip to eliminate the highly skewed elements

What should I do to improve the quality of this mesh ?

Thank you a lot.
Attached Images
File Type: jpg LE.jpg (134.3 KB, 124 views)
File Type: jpg TE.jpg (164.3 KB, 103 views)
File Type: jpg Up view.jpg (71.1 KB, 69 views)
File Type: jpg z-.jpg (210.9 KB, 77 views)
File Type: png setting.png (17.1 KB, 39 views)
aero_cfd is offline   Reply With Quote

Old   September 1, 2017, 10:55
Default Wall normal spacing looks quite large
  #2
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
You are not getting any T-Rex layers at the leading and trailing edges because the T-Rex first step size is as large as or larger than the local surface meshing. T-Rex automatically stops when the marching step size and the lateral size are equal, so it is never getting started in these locations.

I would try using a smaller initial Delta S for the T-Rex walls. Unless this is a really low Reynolds number flow, it looks like it needs to be smaller to resolve the boundary layer anyway.
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   September 18, 2017, 18:05
Default
  #3
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
You are not getting any T-Rex layers at the leading and trailing edges because the T-Rex first step size is as large as or larger than the local surface meshing. T-Rex automatically stops when the marching step size and the lateral size are equal, so it is never getting started in these locations.

I would try using a smaller initial Delta S for the T-Rex walls. Unless this is a really low Reynolds number flow, it looks like it needs to be smaller to resolve the boundary layer anyway.
Hi,

Thanks a lot for your answer, I followed your advice, changed the Delta S to 1e-6 , however as you see the problem at the TE persists , I used Maximum Angle criteria of 165 and Full layers =0 since it's a sharp TE.

Is there something else that can be done to improve the TE area ?

Cheers,
Attached Images
File Type: jpg TE_close.jpg (139.7 KB, 93 views)
File Type: jpg skewn.jpg (202.2 KB, 65 views)
aero_cfd is offline   Reply With Quote

Old   September 18, 2017, 18:34
Post
  #4
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
With a sharp trailing edge like that, you are not going to be able to get a cell with an included angle less than 165 degrees on either side of it. There are several options to get more layers at the trailing edge:
  1. Allow included angles bigger than 165 degrees.
  2. Set full layers to zero. This will allow Pointwise to extrude multiple normals off the sharp trailing edge to improve cell quality.
  3. Use a C-type domain topology to remove the sharp trailing edge angle from the mesh. See tutorial #2 from the Pointwise tutorial manual to see how this works.

Let me know if any of those give you what you want.
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   September 21, 2017, 10:20
Default
  #5
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
With a sharp trailing edge like that, you are not going to be able to get a cell with an included angle less than 165 degrees on either side of it. There are several options to get more layers at the trailing edge:
  1. Allow included angles bigger than 165 degrees.
  2. Set full layers to zero. This will allow Pointwise to extrude multiple normals off the sharp trailing edge to improve cell quality.
  3. Use a C-type domain topology to remove the sharp trailing edge angle from the mesh. See tutorial #2 from the Pointwise tutorial manual to see how this works.

Let me know if any of those give you what you want.

Hi,

Thank you for your reply,

I already used the two first options with no success.
I need tetrahedral cells around the trailing edge for my application, is it possible to get a block around a small portion of the TE with tetrahedral and the rest of the wing with T-REX ?

I tried to split the block created in order to create a hole there then fill that block with tet cells, but apparently Pointwise can't split unstructured blocks ?

Thank you again.
aero_cfd is offline   Reply With Quote

Old   September 21, 2017, 11:32
Default
  #6
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
If you want to force tetrahedral cells around the trailing edge you could put a cylindrical block around that area and fill it with tets as in the attached image.
Attached Images
File Type: jpg Cylinder-Block.jpg (118.7 KB, 115 views)
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   September 21, 2017, 14:04
Default
  #7
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
If you want to force tetrahedral cells around the trailing edge you could put a cylindrical block around that area and fill it with tets as in the attached image.

This is in 2D? how is it done in 3D? create a cylindrical block there and use its exterior surfaces with the T-REX?
aero_cfd is offline   Reply With Quote

Old   September 21, 2017, 14:45
Default
  #8
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
Yes, I did this in 2D just for simplicity, but the same idea works in 3D. Just set the cylindrical domains to a match type T-Rex BC when you extrude T-Rex cells on the main block.
rmatus is offline   Reply With Quote

Old   October 4, 2017, 16:29
Default
  #9
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
Yes, I did this in 2D just for simplicity, but the same idea works in 3D. Just set the cylindrical domains to a match type T-Rex BC when you extrude T-Rex cells on the main block.
I tried what you suggested but the cylinder had highly skewed tetra in it.
I changed the approach and I translated a 2D mesh, and made a a block as shown in the figure , but I still have the same problem when I initialise it.

This mesh is a coarser mesh then the the ones I had before , the domains around re structured created from the translations , and the front and back domains are unstructured.

What can I do to get this block populated with high quality tetrahedral ? I was working on this for a while but can't get what I am doing wrong.

Thank you!
Attached Images
File Type: jpg kewness.jpg (102.3 KB, 80 views)
aero_cfd is offline   Reply With Quote

Old   October 4, 2017, 16:42
Default
  #10
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
Any chance you could share your Pointwise project file (.pw) here? I can think of several possible causes of the problem you are seeing:
  1. Looks like there are some large spacings on the boundaries of the region you are trying to put a tetrahedral mesh on.
  2. There might be inconsistent spacings between adjacent domains (and/or connectors) on the boundary.
  3. Some tetrahedral solver setting preventing it from getting an initial mesh.

For background, why do you want to put terahedral cells in the trailing edge region rather than continue on with hexahedral cells like on either side of that region?

Thanks,
Rick
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   October 4, 2017, 17:09
Default
  #11
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
Any chance you could share your Pointwise project file (.pw) here? I can think of several possible causes of the problem you are seeing:
  1. Looks like there are some large spacings on the boundaries of the region you are trying to put a tetrahedral mesh on.
  2. There might be inconsistent spacings between adjacent domains (and/or connectors) on the boundary.
  3. Some tetrahedral solver setting preventing it from getting an initial mesh.

For background, why do you want to put terahedral cells in the trailing edge region rather than continue on with hexahedral cells like on either side of that region?

Thanks,
Rick
I attached the project file here

I want to have a 3D C_mesh around the wing, with that region with tetrahedral because for my application I want to remesh that tetra region when the TE deforms , and only tetrahedral can be re-meshed efficiently in Fluent .
aero_cfd is offline   Reply With Quote

Old   October 4, 2017, 18:41
Default
  #12
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
Thanks, but when I try to download the file from JustBeamIt it gives the message, "sorry, this download link no longer exists "
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   October 5, 2017, 05:09
Default
  #13
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
Thanks, but when I try to download the file from JustBeamIt it gives the message, "sorry, this download link no longer exists "
I sent you a link in private messages, I hope that one works .
aero_cfd is offline   Reply With Quote

Old   October 5, 2017, 10:24
Default
  #14
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
Yes, the private link worked. Thank you.

The poor mesh quality is caused by large differences in spacings (an order of magnitude jump) between abutting connectors and a large difference spacing between the spanwise (Z) direction and the other two directions (3 orders of magnitude different).

Since you are trying to put an isotropic (same in all directions) tetrahedral grid inside a boundary that is highly non-isotropic there are conflicting constraints that result in poor grid quality.

How do you fix this? You can use Pointwise's T-Rex anisotropic tetrahedral extrusion to solve the first problem, but you will still have problems in its isotropic core region due to the 3 order of magnitude difference in grid edge lengths between the Z direction and the X and Y directions. If Fluent requires fully tetrahedral grid for its adaption then you have to use more uniform grid spacing, which means adding more grid points in the Z direction and thus increasing the cell count significantly.

If you want to try a completely different approach, you could script the TE deformation in Pointwise, which would let you use the more desirable structured, C-topology you want. Here is a webinar that gives a quick introduction to how it works: http://www.pointwise.com/workshops/2...cripting.shtml

Hope this helps.
aero_cfd likes this.
rmatus is offline   Reply With Quote

Old   October 10, 2017, 05:54
Default
  #15
Member
 
Join Date: Aug 2016
Posts: 43
Rep Power: 8
aero_cfd is on a distinguished road
Quote:
Originally Posted by rmatus View Post
Yes, the private link worked. Thank you.

The poor mesh quality is caused by large differences in spacings (an order of magnitude jump) between abutting connectors and a large difference spacing between the spanwise (Z) direction and the other two directions (3 orders of magnitude different).

Since you are trying to put an isotropic (same in all directions) tetrahedral grid inside a boundary that is highly non-isotropic there are conflicting constraints that result in poor grid quality.

How do you fix this? You can use Pointwise's T-Rex anisotropic tetrahedral extrusion to solve the first problem, but you will still have problems in its isotropic core region due to the 3 order of magnitude difference in grid edge lengths between the Z direction and the X and Y directions. If Fluent requires fully tetrahedral grid for its adaption then you have to use more uniform grid spacing, which means adding more grid points in the Z direction and thus increasing the cell count significantly.

If you want to try a completely different approach, you could script the TE deformation in Pointwise, which would let you use the more desirable structured, C-topology you want. Here is a webinar that gives a quick introduction to how it works: http://www.pointwise.com/workshops/2...cripting.shtml

Hope this helps.
Thank you a lot for your help, one last question, I didn't uite understand what you meant by scripting the TE deformation, you mean create different meshes for each TE deformation ?

Cheers,
aero_cfd is offline   Reply With Quote

Old   October 11, 2017, 23:01
Default
  #16
Senior Member
 
rmatus's Avatar
 
Rick Matus
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 116
Rep Power: 15
rmatus is on a distinguished road
Yes, you can script both the geometric deformations and the regeneration of the mesh using the Glyph scripting language.
rmatus is offline   Reply With Quote

Reply

Tags
mesh 3d, pointwise, t-rex bcs

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Ffd_control_point_2d feiyi SU2 4 September 30, 2019 13:42
Wing FSI simulation: Shell elements or 3D solid body? frossi CFX 3 June 15, 2016 21:02
Ansys SIG$ILL error loth ANSYS 3 December 24, 2015 06:31
Highly skewed and inverted volumes in wing mesh makaero FLUENT 0 December 8, 2009 20:32
CFX4.3 -build analysis form Chie Min CFX 5 July 13, 2001 00:19


All times are GMT -4. The time now is 22:16.