Solid Element Type Study 1

[davemechuk]

For those whom are lazy:
Tet linear elements require 15-50 times the number of nodes for a converged solution and still provides a margin of error of 1% which is 5-10 times greater than the other elements. Is this right?

Full story:
I've performed a fairly thorough mesh convergence study for the following four solid element types within ANSYS:

Hex Linear
Hex Quadratic
Tet Linear
Tet Quadratic

I have obtained results that I did not expect and hope that someone could do two things for me:

1. Explain why this is so (read on)
2. Point me to any literature that confirms/investigates this (I have had a quick search with no sucess)


---------------------------------------------------------------------------------------------------------
The study:

I have modelled a simple cantilever beam as a solid. Dims: L=15mm, d=5mm b=10mm. I progressively changed the element size from 2.5mm to 0.02mm (a total of 66 iterations per model).

I have quried only the bending stress at 7.5mm away form the load applied to the cantilever end.

The results:
The Hex (Lin and Quad) elements and Quadratic Tet elements all converge fairly quickly. Large element sizes (2.5mm) start off around 1% away from the expected stresses. The Tet linear element starts off with stresses 40% smaller than expected. The following performances are observed with the element converging the 'quickest' listed first:

Hex Quadratic - Converge at a mesh size of 1.35mm (2,100 nodes) within 0.1% of the converging solution, with a margin of error of 0.2% to the expected result from the simple hand calc.

Hex Linear - Converge at a mesh size of 0.8mm (2,200 nodes) within 0.1% of the converging solution, with a margin of error of 0.2% to the expected result. Note the mesh SIZE is much smaller but the NODE count is only 6% greater.

Tet Quadratic - Converge at a mesh size of 1.15mm (6,700 nodes) within 0.1% of the converging solution, with a margin of error of 0.1% to the expected result.

Tet Linear - This only just converges at a mesh size of 0.225mm (100,000 nodes!!) within 0.1% of the converging solution, with a margin of error of 1% to the expected result.


Dave, Msc(Eng), AMIMechE
Graduate Stress Engineer
(3 Years left for Chartership!)

 

[burningDiesel]

Sounds right, in some cases, lineair tets never converge. In other cases, they show to be converging, and if you refine further, diverge again. In general these elements are to be avoided, especially since you can just use quadratic tets.
If you see something modeled with linear tets, you can disregard the work 'cause they don't know their stuff. Only for very specialised things you might want to use them (element deletion, extreme deformation, ...).
In general, they are too "stiff".

For the hex, did you check reduced/full integrated elements?

The fully integrated quadratic hex can also show wierd behavior in bending (especially with incompressibility).
Fully integrated linear hex can exhibit shear locking and volumetric locking, while reduced integration can have hourglassing. Ansys & Abaqus have ways to battle this with special element types.

Again, in general, reduced integration quadratic hex > everything.
quadratic tets come second, but are more expensive

 

[davemechuk]

Very helpful thankyou.

I believe I left the default on (Full integration), I was wondering why my shear loads were acting up, I was aware of shear locking and issues with incompressibity of elements, just didn't know how to battle it. I take it this is why my shear stresses are incorrect.

Thanks for your time, the first decent reponse I've had on here!



Dave, Msc(Eng), AMIMechE
Graduate Stress Engineer
(3 Years left for Chartership!)