CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Problem with first prism layer (http://www.cfd-online.com/Forums/ansys-meshing/65825-problem-first-prism-layer.html)

Twix June 27, 2009 04:15

Problem with first prism layer
 
Hi,

I have problem with creating prism layers in ICEM . When I decreasing first layer height I get this message:

** loop distorted (element size = 5.30063e-007 < 7.41331e-006)
trying simple triangulation for this loop
or
** elements distorted (w = 30.8446 > 9)
trying simple triangulation for this loop

or something with err=7 and meshing failed. What I have to do to decrease high first layer? Please help me.

Regards

PSYMN June 29, 2009 13:54

Tri-tolerance...
 
My guess is that you have reduced the hight of your prism down to lower than the geometry tolerance. Behind the scenes, your nurb geometry is facetized for projection, if these facets are too large and your prism is too fine, you can run into issues like this.

To fix it, try reducing your tri-tolerance. This is a global setting. It defaults to 0.001, but try 0.0001 or finer to see if you can get this to work. You will need to regenerate the tetra with this smoother geometry before you can try out the prism again...

Simon

PSYMN June 29, 2009 14:07

Surface Meshing...
 
Oh wait, that last guess was assuming you were getting issues running prism on a tetra volume mesh... I guess I didn’t read your error carefully enough. Actually, these errors look like surface mesh errors.

When you adjust your prism height settings and then generate a surface mesh (or generate a prism mesh from geometry with the surface mesh settings set to patch dependent and the volume mesh settings set to something bottom up like Delaunay) the surface mesher can use these initial heights set on curves to control an offset from the curve boundary (quads around the perimeter of each surface). This is running into trouble and causing the “loop” to fail. Instead of paving across this loop, it tries a “simple triangulation”; this is when it just connects the nodes on opposite sides with long or large triangles. It is rarely suitable for further volume meshing and may even fail completely on some loops.

Since you can’t get a nicely closed surface mesh, the bottom up Delaunay or advancing front also fails and then prism fails…

If you mean to use a surface mesher with patch conforming mesh, you really need to setup more carefully. Try one of the surface meshing tutorials. Get the surface mesh right first, then generate the tetra mesh as a separate step and then run prism only after checks and smoothing.

If you just wanted a regular ICEM CFD tetra prism mesh, check your settings. Make sure your tetra/Mixed method is set to octree. I would still recommend getting the tetra mesh first and doing all your checks and a bunch of laplace smoothing. You could even replace the octree volume mesh with the Delaunay or advancing front mesh before running prism.

Twix July 6, 2009 16:31

Hi

Thank for your replay. I try some of Your suggestion but none of them help me, but I read this forum and I found Your post about IGES and STEP files ( I use IGES) and I change geometry file I import and its working, I decreased my first prism layer. Thank U very much.

Regards


All times are GMT -4. The time now is 07:00.