CFD Online Logo CFD Online URL
Home > Forums > Mesh Generation & Pre-Processing Software > Pointwise & Gridgen

Convex T-Rex meshing

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

LinkBack Thread Tools Search this Thread Display Modes
Old   November 17, 2016, 05:45
Default Convex T-Rex meshing
New Member
Join Date: Jul 2012
Location: Norway/Germany
Posts: 13
Rep Power: 13
Drunken_SheeP is on a distinguished road
So I am trying to mesh an 2-D iced airfoil. When there is ice on on the leading edge the geometry becomes quite complex with a lot of convex and concave curvature. Until now I have used quite successfully a structured mesh to capture these geometries. Using the hyperbolic extrusion, I typically had very little problems.

However, I would like to test out the suitability of T-Rex meshes. I think it could make my meshing process much faster and robust. Unfortunately, I do not have too much experience using T-Rex meshes so far. The mesh on a clean airfoil looked quite good and performed well. However, for the iced geometries I am not quite happy with the resulting grid (see below). In particular, I think that the mesh quality in the concave areas is not optimal. I am particularly concerned about the area where two converging grid layer lines meet.

I have been trying to fix this by changing some of the smoothing parameters but without result. But of course I have no idea which parameters to tweak

I'd highly appreciate it if somebody had some advice!

€dit: The title should say concave of course
Drunken_SheeP is offline   Reply With Quote

Old   November 30, 2016, 15:43
New Member
Join Date: Jul 2012
Location: Norway/Germany
Posts: 13
Rep Power: 13
Drunken_SheeP is on a distinguished road
Anybody some suggestions?
Drunken_SheeP is offline   Reply With Quote

Old   November 30, 2016, 22:46
Senior Member
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 161
Rep Power: 15
tcarrigan is on a distinguished road
The smoothing parameters in 2D T-Rex aren't going to help in this case. The smoothing parameters are used when you have different initial spacings specified in the T-Rex Boundary Conditions tab for different connectors and helps to blend the extrusion. In your case, I assume you are using a single initial spacing off the wall.

Looking at your images it looks like you have the Full Layers parameter set to a rather high value. I can tell because some of the anisotropic triangles have pushed passed isotropy. Instead, set full layers to just 1 to turn off multiple normals at convex corners.

But the biggest thing to consider is adjusting your grid point spacings around the airfoil. As you know, with T-Rex you are advancing elements off the surface and at some point they will collide with another front. To improve the element quality in the collision regions, you'll want to ensure that the surface spacing (connector grid spacing in your case) is similar inside convex regions. By keeping the surface spacing consistent, when the layers begin to collide they will be of similar area.

It's best not to use T-Rex like the hyperbolic extrusion tool by trying to push the entire front to the same number of layers. The advantage of T-Rex is that the front can stop locally due to quality criteria being violated or because the elements have already reached an isotropic state. This means that you will end up with a different number of layers around the airfoil, but that's generally ok as they'll more naturally stitch with the isotropic tri farfield mesh.
Travis Carrigan
Manager, Business Development
Pointwise, Inc.
tcarrigan is offline   Reply With Quote


airfoil, icing, t-rex

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
[ANSYS Meshing] only automatic meshing works, kazra ANSYS Meshing & Geometry 2 February 23, 2017 11:38
[Gmsh] 3D coil mesh: can't create the volume? RomainBou OpenFOAM Meshing & Mesh Conversion 3 July 18, 2016 05:09
[Gmsh] Vertex numbering is dense KateEisenhower OpenFOAM Meshing & Mesh Conversion 7 August 3, 2015 10:49
[blockMesh] Meshing no convex domain using spline or polyLines loic_d OpenFOAM Meshing & Mesh Conversion 1 April 6, 2015 07:18

All times are GMT -4. The time now is 13:50.