Nodal vs Elemental Stresses - Revisited
Carl Howarth
We had a discussion of nodal vs elemental stresses a few months ago that
was mostly theoretical. My question now is of a practical nature.
Assume you have a simple beam in 3 point bending, which is meshed with
brick elements. This model has 3 bricks through the thickness x 10
bricks wide x 100 bricks long. I've seen that a plot of maximum
principal stresses will indicate that the elemental stress is lower than
the nodal stress, particularly at the surface of the beam. This is
logical because the nodes at the point farthest away from the neutral
axis will experience higher stress.
The question is - which stresses actually represent the stresses in the
part? I have run simple analyses and compared them with hand
calculations, and have found that the elemental stresses more
realistically represent the stresses on the beam.
Is this true always? When should one consider looking at nodal
stresses?
The reason that I ask is that an analysis I completed recently shows
failure in the part, while a prototype test showed that the part will
survive. I spent signicant time ensuring that this model accurately
reflects the geometry, loading and material properties, and I need to be
absolutely sure that I am interpreting the results correctly.
Thanks in advance for any insights.
Best Regards,
Carl Howarth
Christopher Wright
<howa...@mindspring.com> wrote:
>The question is - which stresses actually represent the stresses in the
>part? I have run simple analyses and compared them with hand
>calculations, and have found that the elemental stresses more
>realistically represent the stresses on the beam.
Nodal stresses are extrapolated If your mesh is fine enough the
extrapolation becomes more accurate and nodal and element stresses are
equally accurate. You already discovered the biggest reason for
considering nodal stresses--stress concentrations occur at surfaces, so
you need accurate nodal stresses to calculate stress concentration effect
accurately.
--
Christopher Wright P.E. |"They couldn't hit an elephant from
chris!w...@skypoint.com | this distance" (last words of Gen.
___________________________| John Sedgwick, Spotsylvania 1864)
http://www.skypoint.com/~chrisw
Timo de Beer
Carl Howarth wrote:
>
> The reason that I ask is that an analysis I completed recently shows
> failure in the part, while a prototype test showed that the part will
> survive. I spent signicant time ensuring that this model accurately
> reflects the geometry, loading and material properties, and I need to be
> absolutely sure that I am interpreting the results correctly.
>
Testing for failure, specially when considering brittle materials, is
bound to give a large spread in results even when using supposedly
similar test pieces. Combined with the problems associated with
accurately determining the failure limits of the material used, this
makes it very unlikely that your analysis would ever predict failure
correctly (although I know that some software vendors object to this
statement).
Therefore I don't think that it is possible to obtain any answer to your
original question about stress points from the observed lack of failure.
Timo de Beer
Carl Howarth
Thank you for the response. In this case, however, the material is a HSLA50
steel, with a predicted yield of about 50,000 psi. I wouldn't attempt to
model ceramics or highly alloyed metals that exhibit brittle behavior, as I
know enough to know that there is much more involved. I'll leave that to the
PhD's.....
Regards,
Carl Howarth
Keith J. Orgeron
Consider these subtle details:
- Did you select the largest max. princ. stress shown, or the mid span value?
- (I'm sure you distributed the loads/BC's along the 10" edges.)
- Did your 3 point loading include edge effect load reductions?
- Did your BC's include allowance for one edge free to slide?
- (Your BC's did not exactly reflect the calcs which assumed mid-thickness BC's.)
- Did your prototype test setup allow frictionless axial movement of one end?
- Was your plate very thin, and thus had large deflection?
- Did you use a large displacement solution for the FEA or your hand calcs
- Others...
[The exact subject is addressed later in this message. Though you've
specifically inquired about elemental/nodal stresses, a much more comprehensive
coverage of "model validation/verification" is really quite in order... but only
briefly noted here.] I guess that your prototype test involved a single overload
event defining failure? Or was it a high or low cycle fatigue test? Even so,
the definition of "failure" must be strictly defined in order to select and
complete the material model and other solution parameter sets required for an
accurate simulation. At least then you have a fighting chance to validate/verify
your simulation to the test results which also inherently contain a certain
statistical spread of values.
For instance, overload of the HSLA 50 material (which is a fairly ductile steel)
will require a nonlinear (NL) material model, for which there are many with
different degrees of curve matching and even basic, theoretical assumptions (such
as isotropic, kinematic or mixed/hybrid schemes.) Your mesh, choice of element
and solution formulations, solution convergence parameters, etc. all play a part
in a more or less accurate solution.
For high cycle fatigue, a linear solution would typically do fine, since this
does not involve any plasticity. However, for a low cycle fatigue duty, the
stress cycles could approach or surpass the yield strength.
Ultimately, your decision of which stress display to compare with test results is
also important. For ductile steels, the effective Von Mises (combined) stress
display has been shown to be very representative. You mention that the elemental
maximum principle stress plots were closer to your hand calculations... but the
nodal (surface) stresses should have matched better. Accuracy can also depend on
your choice of element options, as in nodal "compatibility." If your FEA code
supports a "nodal compatibility not enforced" feature, then this should be used,
as it has been shown to yield more accurate stiffness values for linear (lower
order) elements such as your 8 node bricks. A mesh convergence study should also
be performed for this simple configuration, say of maybe two or more mesh
densities.
By addressing each an every "model idealization" (mathematical assumptions made
to easily represent real phenomenon) used in creating your simulation model and
then, every "numerical approximation" (mesh, solution method, etc.) used in the
solution, you can virtually quantify your overall "simulation accuracy."
Ascertaining this accuracy is a form of "validation," and correlating your
interpreted simulation results to your test results can be a form of
"verification" of your simulation approach.
Hope this wasn't too long winded,
Keith.
Carl Howarth
As usual, thanks for your response. I am quite certain that boundary conditions are
representative - that particular model was run as linear, although deformations
approaching the steel thickness were found. I suspect that the answer as to why my
model predicted failure and the prototype was fine lies in the fact that my analysis
was linear. BTW, the test was a single load cycle.
To solve my question of nodal vs elemental stresses, I've run a number of analyses on
simple geometries and compared stresses with hand calculations. I've found
universally that the hand calculated answer (for a number of bending problems)
matches very closely with the nodal stresses from the model. In fact, the the nodal
stresses have been within 1 or 2% of the hand calculated stresses. Even with
extremely fine meshes, however, I have found that the predicted elemental stresses
are always too low. Typical differences between mesh and nodal stresses have been on
the order of 50% to 25% (depending on mesh size). The elements that I used were
bricks, and the deflections in the analysis were very small. I am very careful about
element distortions.
Given this experience, it appears that I will try to examine nodal stresses in the
future.
Best Regards,
Carl Howarth