Cheng,
I modelled an ultrasonic system in Comsol for my PhD. The system was a
bolt clamped piezoceramic transducer with a steel backing section and
an aluminium horn. The system was designed to oscillate at resonance.
My thesis title is:
Modelling of an ultrasonically assisted drill bit, 2008, Loughborough
University.
Here is an extract which might help you:
*****
Guidelines and considerations for transient analysis
====================================================
Element Size, Shape and Order
-----------------------------
(Wasley 1973) states that for Hooke's law to apply to dynamic wave
propagation
problems, the size of each element under consideration must be less
than a tenth of the size
of the wavelength (for all frequencies considered) within the body.
Further to this,
(Abboud, Mould et al. 1998) documents that 10 elements per wavelength
generates a
numerical dispersion error of about 3% whilst 20 elements per
wavelength reduces the
numerical error to less than 1%.
The elements' geometrical aspect ratios are also pertinent to
numerical accuracy (Becker
2004). (Abboud, Mould et al. 1998) states that the finite element
aspect ratio should remain
close to one, but can safely reach 2 or 3 to accommodate geometric
constraints and (Bathe
1996) sates that, whilst employing Implicit integration schemes to
model wave
propagation, non-uniform meshes with low or high order elements may be
used. Comsol
Multiphysics automatically calculates the mesh quality q (Comsol
2006c), and guidelines
(which are dependant on the element types employed) are given to
ensure numerical accuracy.
If Poisson's ratio effects (i.e. lateral stress gradients) are to be
modelled accurately in long
thin bars, (Abboud, Mould et al. 1998) states that a minimum of 6
element node points are
required over the width of the bar for the effect to be resolved.
In addition, (Becker 2004) states that if the geometry under
consideration has complex
boundary geometries, higher order elements should be employed, and
(Abboud, Mould et
al. 1998) states that, since vibration propagates throughout a FE
model, the same degree of
discretization should be maintained throughout the mesh to avoid
directionality and
spurious internal reflectors.
Finally, (Becker 2004) states that near sharp stress gradients,
elements must be of a smaller
size, and they must increase in size gradually to ensure that the
degree of approximation is
spread across the FE mesh.
Maximum time step allowed
-------------------------
In order to ensure that each time step is accurately integrated, the
time step Dt employed
must be sufficiently small. (Abboud, Mould et al. 1998) states that,
when analysing wave
phenomenon, a time step smaller than 1 / 10 of the time period T of
the highest frequency
of interest is required. (Bathe 1996), however, recommends that Dt<=T/20 .
If this constraint is not adhered to, it is likely that the
numerically derived system vibration
will be inaccurate with respect to either or both vibration period and
amplitude decay
(Bathe 1996).
The time step size determines the maximum oscillation frequencies that
the numerical
system can model, although any high frequency oscillations (higher
than anticipated and
accounted for) present in the model will more likely be portrayed
inaccurately.
A good approximation to the maximum significant frequency component
exhibited by a
system (if unknown) is 4Žw where w is the system excitation frequency
(Bathe 1996).
Maximum error tolerance allowed
-------------------------------
The materials of interest in this study exhibit extremely low levels
of damping around the ultrasonic frequencies and amplitudes
of interest. Any damping modelled during FE analysis must be
satisfactorily characterised
in order that its effects remain consistent.
It is assumed (for sake of argument) that a simple bar, vibrating in
its fundamental
longitudinal resonant mode, can be modelled as a single degree of
freedom system
incorporating a mass, and a spring and viscous damper arranged in
parallel.
The decrement in vibration amplitude Dx over a single time step Dt, at a
given vibration amplitude and due to viscous damping alone, can be
written.
As such, if a FE model is to exhibit a specified Q factor (which
relates to the damping in the system), it must be solved to an accuracy
that, at the very minimum, resolves Dx accurately at the amplitudes at
which the model
oscillates.
There are two assignable tolerance values incorporated into Comsol
Multiphysics' time
dependant solver. These are the Absolute Solution Tolerance, and the
Relative Solution
Tolerance.
It must be noted that since the relative tolerance setting is
dependant on the
instantaneous magnitude of the displacement at the node being
considered; careful
selection of this value is required. No accuracy at all is achieved
when the solution
tolerance is greater than the displacement magnitudes calculated, and
it must also be noted
that the accumulated global error can be larger than the sum of the
local errors. Having
said that, (Comsol 2006c) states that the solver's error estimate is
overly pessimistic and
that the true global error is of the same order of magnitude as the
local error.
As can be seen from the above formula, the solver favours the least
stringent tolerance, and
in the oscillatory conditions under investigation, the controlling
tolerance criteria will
alternate between the absolute and the relative tolerance settings.
This occurs because the
displacement magnitudes within the bodies under consideration will
oscillate between
positive and negative displacement values, sometimes achieving large
displacement
magnitudes, and sometimes attaining almost zero levels of displacement.
*****
Another note is that you will likely have to assign damping
coefficients carefully for a transient analysis...
Regards,
Peter Thomas
Post by gruenstWhich solver did you use? Did you try different solvers?
Any information about your meshing? Could you upload your file in the
file section? Does your programme work with different settings?
Sorry, only more questions...
Post by yc_001Hi all,
I'm so stucked in this convergence problem and can't move further for
2 weeks..It's so frustrating.
I'm doing a piezoelectric modeling, in my model I give a sin voltage
as an excitation and would like to observe the result in time domain.
The frequency is 6000Hz so one period is 1.67e-4s, I would like to
observe the model in two periods so I set 3.3e-4s.
So I set the time step as 0:1e-5:3.3e-4, relative tolerance as 0.01,
absolute tolerance as 1e-15. I solved the model, and everytime I got
Time 1.6384e-008: (the value was keeping changing but it always
stucked in some value of power 1e-8)
Nonlinear solver did not converge.
Last time step is not converged.
And of course I tried to solve the problem, by changing the absolute
tolerance, since COMSOL says the absolute tolerance should be one
power smaller than the displacement. And I tried to change the time
step, from 1e-4 to 1e-10, and it still did't work. And now the error
message is still keep coming..
Any suggestion is warmly welcome. Thank in advance.
Regards,
Cheng