Simulation Mesh Size Absolute

[jeang32]

Hello,

I have a "board" which dimensions are 110 x 300 x 3cm. I am trying to generate a mesh fit for analysis.
When using Absolute size.
a. If the size setting is set to 10mm, I get 6 tetrahedral elements in the thickness section.

b.  If the size setting is set to 12mm, I get 2 tetrahedral elements in the thickness section

I was expecting 4 ? In fact I am unable to find the absolute Size thickness settings which would lead to 4 elements in the section....
Can you pls explain what is actually happening ?

2. From reading I understand to get meaningfull results from this analysis of deformation of force/load applied in the direction of the thin section, in parabolic element order, I would need at least 6nodes.
This is would be achieved by the 4tetrahedral, correct ? 
6 tetrahedral in a section is slow to solve and would like to avoid it as a starting point for an adaptive mesh analysis which takes too long.

Thank,
Jean P.

[todd_alford]

Hi @jeang32,

This looks to be a little bit of a misunderstanding and an issue as well, so let me explain what we see in the first image, to bring some clarity.  The element size is set to 10 mm, the thickness of the board is 30 mm.  So we would expect to see 3 elements across the thickness.  I believe you may be counting elements that are side by side, if you look at a single triangle (the side of one element).  It is mirrored back and forth to cross the board for a total of 3 elements to cross the board. 

If you start at 1 point, and cross the board there are 4 nodes (each intersection and the endpoints that define each side of the board).  So to get to 6 nodes you would need 5 elements.  elements*element height should equal our thickness so 30/5 gives us an element size of 6 mm.

In your second picture it is slightly misleading, you only have one element across the thickness (a single triangle has points on both sides of the board).  This is where we run into some nuances of meshing, you should have at least 2 elements across the thickness but while the mesher is trying to maintain similar size elements to get across 30 mm we would only be at 24 after 2 elements and a third element will be half the size of the other two.  We could play some games and get that to work, but it would be more appropriate to select a size that would easily cross the thickness with an integral multiplier.

Does this help?

Thanks,

Todd 

[John_Holtz]

To elaborate on Todd's answer, the node count that he referenced is if using linear elements. Two linear elements through the thickness would give 3 nodes across the thickness, like this:

You mentioned parabolic elements (which is the default in Fusion). Two parabolic elements through the thickness would give 5 nodes across the thickness, like this:

But you simply cannot compare the node count through the thickness. Linear elements give a linear distribution, where as parabolic is able to calculate a higher order distribution. Two parabolic elements with 5 nodes through the thickness may be as accurate as 6 or 7 linear elements with 7 or 8 nodes through the thickness (just an example off the top of my head; I do not know the exact comparison).

What really counts is the number of elements/nodes through the stress gradient. This article is for a different product (Simulation Mechanical), but it provides some more details about the concept of elements through the stress gradient. See Thin parts can have inaccurate results when using brick elements. With Fusion, substitute "solids" or "tet elements" in place of "bricks" in the article.

 

[jeang32]

Many thanks for the response.

What you are showing with the 5nodes across is what I am after. However, I am unable to achieve it.
I understand from @todd_alford message that 12mm can lead to non integer division.

However,

1. 15mm leads to 3 nodes across (see bottom picture).
2. I cannot find a thickness setting for this 30mm slab which leads to the mesh with 2 tetras across and 5nodes.

[John_Holtz]

Hi @jeang32

I do not know why meshing a 1100 x 3000 x 30 mm body with a mesh size of 15 mm does not create 2 elements through the thickness. 1100 x 1000 x 30 mm with a mesh size of 15 mm does create 2 elements through the thickness. It does not make sense -- unless you are a computer or a developer .

My only suggestion is to break the 1100 x 3000 body into 3 sections. That may give you 2 elements through the thickness with a mesh size of 15 mm.

[Anonymous]

@jeang32,

Have you tried turning down your aspect ratio?

[jeang32]

The split body worked just fine. thanks @John_Holtz

@Anonymous, I had tried but it did not change the # tetras across. I gathered this was due to the fact that the smallest aspect ratio  is 4... And perhaps not low enough to increase the # tetras in the cross section.

Jean