Solid Meshing Problems

[Inv_kaos]

I am having increasing problems with the solid meshing, the attached example has only just finished as I am writing this, it took about 2-3hours. Most of the mesh is coarse with refinement points as indicated, it solves in a fraction of the time it takes to mesh which is not right.

If I use lots of refinement points with a small radius, will it mesh slower than if I use fewer refinement points and larger radius, essentially giving me the same mesh field?

I notice that my CPU and RAM usage is very minimal so I don't know why it takes so long to grind through closing the voids. Is there anything I can do to speed it up? I can't change the mesh size because I need at least 5 elements through the thickness for my fatigue checks.

Cheers

[John_Holtz]

Hi,

Have you tried the option to create a layered mesh? This would give better control over the number of elements through the thickness, and it does not perform the solid meshing that is taking so long for you now. From the documentation:

This mesh will create a user-entered number of solid elements through the thickness. Since the number through the thickness is applied throughout the part, this option is suitable for thin parts with relatively constant thickness. 

It is hard to see what the junction between the nozzle and vessel looks like. If there is a fillet, you may need to make your model an assembly where the nozzle and vessel are one part and the fillet (weld) is another part. Use the layered mesh for the vessel and regular solid mesh for the fillet. Then activate the smart bonding to connect the fillet to the unmatched mesh of the vessel/nozzle.

Here are a few items related to the solid meshing:

1. Even though your surface mesh may have 5 elements "through the thickness", that only occurs on the symmetry plane. There is no control for the solid meshing through the thickness once it gets aways from that edge, so there is no guarantee that you will have 5 elements through the thickness at all locations.
2. The time it takes to solid mesh is not directly related to the number of refinement points. Solid meshing is only dependent on the surface mesh. Technically, the surface meshing will be faster with fewer refinement points, but I doubt that you will see much of a difference in this model.
3. The solve time is essentially pre-determined by the mesh. Everything is known: N equations with N unknowns. The solver does not change the model to make it better. (The exception is when some type of surface contact is included. That is an iterative solution that requires an unknown number of iterations to converge.) On the other hand, solid meshing is filling a volume with an unknown number of elements of unknown shape, and it is adjusting the shape of the elements to meet the quality specified. So it takes an unknown number of tries to fill the volume. Not to say that there is not room for improvement in the solid mesher, but that is generally why it can take longer to mesh than to solve.

[Inv_kaos]

Thanks John,

I had not tried layered mesh but it almost is exactly what I need. What I don't like, it mitres the mesh at any change of direction instead of keeping it square, additionally it will taper the geometry to suit any small changes in thickness. This creates a problem for me, particularly when bonding to other solids.

It would be good if the number of elements through the thickness would follow tapers and changes in thickness, just like a swept mesh but it fails pretty miserably when I try. Unfortunately when I include my pad and fillets (as solids) to the neck and shell (layered) I get a lot of gaps opening up, plus the tapering of the mesh in regions where I need to measure my stresses. I think layered mesh could be really good with some feature enhancements for complex geometry (follow taper, variable elements through thickness in built up regions, square transitions at large changes in direction, etc).

Anyway I am back on full solid meshing, current mesh I put on at lunch yesterday, left run overnight and it is still going 24hours later. I can live with meshing taking longer than analysing but I don't have the liberty of waiting this long for a relatively simple simulation. Does Femap work with the Algor solver? I might be able to do it another way.. Have a look at my log file and see if anything looks wrong. I will rerun with all tet and see if it is quicker.

My Log File:

[code]

Length units used in the log file are modeling units: mm
Hexagen - Automatic Brick Mesh Engine
Version 2012.1, 15-Jun-2011
Copyright (c) 2011, Autodesk, Inc. All rights reserved.
PROGRAM WILL USE THE FOLLOWING FILES:
Input: C:\FEA\JN2781\2781-F-09.FEM
Output: C:\FEA\JN2781\2781-F-09.FEM
COMMAND LINE:
C:\Program Files\Autodesk\Algor Simulation 2012\SOLIDX.exe -b=0 -o=2 C:\FEA\JN2781\2781-F-09 -ds=1 -f=1 -u=13 -c=2 -t=1 -progress_pipe=4
TYPE OF OPERATION:
Meshing only surface defined by part 1
Generating bricks, wedges, pyramids and tetrahedra elements
Automatically minimizing aspect ratio of solid elements
ERROR NUMBER 104:
Solid meshing is aborted by user.
DIAGNOSTICS:
Patched loops : 0 of 0
Uncovered layer surface : 7.3%
Built 0 filler elems ( 0.0% of vol.)
Elements removed : 7406 [0,1253,6153] (vol:5340847.632487)
Pyramid level : 3
Hgen-tetra level : 5.2
ORIGINAL MAXIMUM WARP: 3.3 DEGREES.
ORIGINAL MAXIMUM LENGTH-BASED ASPECT RATIO : 7.6
FINAL STATISTICS:
Still have: 3189 nodes; 11206 lines; 8086 triangles
Elements built (4,5,6,8 noded): 473180 ( 203505, 93777, 10786, 165112 )
Volume (4,5,6,8 noded %): 88461065.057169 ( 4.59, 5.94, 1.39, 85.09 )
Length ratios (avg) 15.8, 4.0, 2.5, 2.1
Length ratios (max) 324.5, 87.2, 14.6, 17.9
Aspect ratio: unconstrained ( 13.5, 3.9, 1.6, 1.5 )
Average aspect ratios: ( 1.5, 1.3, 1.1, 1.0 )
Number of restarts: 0
Elapsed time: 23 hours 37 minutes 59 seconds

[/code]