Questa è una vecchia versione del documento!
To enter the reserved areas of the site, you must first register at the link.
Lecture Notes
Shared terminal lab
Videos
Various stuff
Sparse material
Hex20profile model
-
Wall thickness 2mm.
Wall scale local reference system: direction 1 (red), axial; direction 2 (green) in cross section, along the wall; direction 3 (blue) normal to the wall.
Adhesive layer thickness 0.5 mm, elastic isotropic material with E=1000 MPa, ν=0.3.
A Phoney monocoque chassis
Properties
Suspension link trusses
Solid circular beam sections, ø12mm, aluminum.
Essentially rigid with respect to other chassis structures.
Rear framework
Hollow circular section beam, aluminum.
Main structure: outer diameter ø40mm, wall thickness 1.8mm.
Stiffeners: outer diameter ø30mm, wall thickness 1.2mm.
Composite monocoque
Thicker backbone: 1.8mm aluminum sheet, 25.4mm aluminum honeycomb 3003, density 5.2 lb/ft^3
(hex-3003-td.pdf),1.8mm aluminum sheet.
Directional homogeneization is employed for the honeycomb, i.e.
$$G_{zx} \approx G_{zy} \approx \frac{2}{\frac{1}{G_{zx}}+\frac{1}{G_{zy}}}$$
Thinner panels: 1.8mm aluminum sheet, 6.35mm same aluminum honeycomb, 1.8mm aluminum sheet.
Frontal shock absorber support plate: provisionally as thinner panels, to be defined based on shock.
Sway (anti-roll) bar
outer diameter ø25mm, wall thickness 2mm, extremely stiff (Super-alloy Z, E=E_steel*1e4, nu=0.3); it may be mechanically isolated at need by deactivating one of the connecting elements to the wheel hub carriers.
Such a “deformable but extremely stiff” linkage modeling should be discouraged in favor of an actual kinematic constraining – i.e. an MPC, since excessive stiffness badly impacts the system matrix condition number (or the integration time step, in the case of explicit dynamic simulations); nonetheless, it allowed for a very straightforward implementation.
Inertial elements modeling
The following spreadsheets are used in defining the equivalent rectangular cuboids for each inertially relevant rigid body:
engine,
wheel assemblies.
The driver inertia is modeled through an 80 kg steel bar spanning roughly from the sternum to the pelvis.
Frontal crash absorber collapse loadcase (inertia relief)
At the element faces belonging to the crash_absorber_bearing_area set (an approx. 155×320 mm area at the front bulkhead), a 25 psi = 0,172 MPa distributed pressure is applied which is due to the honeycomb absorber crushing (see datasheet).
How to set a damped response
In order to include a small degree of structural damping (eg. 1% of the critical value) into a MSC.Marc/Mentat harmonic response calculation, the following steps may be followed:
enter the menu MAIN → MATERIAL PROPERTIES → MATERIAL PROPERTIES;
preemptively define a modulating table 1/ω
menu TABLES, NEW → 1 INDIPENDENT VARIABLE
define NAME as modulate_stiffmatmult
set Indipendent variable v1 TYPE as frequency
define table through FORMULA and type 1/pi/v1, i.e. $g(f)=\frac{1}{\pi f}$
go back to MAIN → MATERIAL PROPERTIES → MATERIAL PROPERTIES by hitting RETURN;
select the various model materials, and for each of them enter the submenu STRUCTURAL → DAMPING and activate DAMPING;
leave alone the MASS MATRIX MULTIPLIER value (0 is ok, otherwise some “structural” damping will be associated to rigid body motions),
define a STIFFNESS MATRIX MULTIPLIER equal to the desired fraction of the critical value, namely 0.01,
set a frequency modulating function, namely TABLE, by hitting the TABLE button on the right of the stiffness matrix multiplier value;
select the just defined modulate_stiffmatmult table as the modulating one, hence hitOK and OK again to return back at the material properties menu
in this way, I defined damping as a function of the $\alpha$ e $\beta$ coefficients introduced by the Rayleigh proportional damping model, with zero $\alpha$ and hence no contribution of the mass matrix. In particular $\zeta = \frac{1}{2}(\frac{\alpha}{2 \pi f}+2 \pi f \beta)$ with $\alpha=0$ and $\beta= 0.01 \cdot g(f)=\frac{0.01}{\pi f}$, from which $\zeta=0.01$ as desired.
enter the MAIN → JOBS menu and create a copy of the undamped harmonic response job by hitting the COPY top left button and by setting a new job name;
enter the job PROPERTIES menu, and reach the ANALYSIS OPTIONS submenu; activate the COMPLEX DAMPING options within the dynamic harmonic section, and then exit withOK
Enter the JOB RESULTS submenu and deactivate Stress, Equivalent von Mises stress
substitute them with the AVAILABLE ELEMENT SCALARS
Equivalent Real Harmonic Stress , layers MAX & MIN
Equivalent Imag Harmonic Stress , layers MAX & MIN
the REAL HARMONIC e IMAG HARMONIC stress resultant equivalents for the beam elements, DEFAULT layer, and the Beam Orientatio Vector
insert from the AVAILABLE ELEMENT TENSORS block
Real Harmonic Stress , layers ALL
Imag Harmonic Stress , layers ALL
run the simulation as usual with RUN → SUBMIT
open the post file as usual with OPEN POST FILE (RESULTS MENU)
The deformed shape may be visualized according to a given phase within the oscillation cycle (see also the DEFORMED SHAPE SETTINGS menu); in the absence of damping the fase was limited to the 0° and 180° values, cases these that may be represented with the bare variation in sign of the stress and displacement components to be monitored.
Please note that the real component has a 0° phase ($\cos(\omega t)$ modulation) whereas the imaginary component has a 270° phae ($-\sin(\omega t)$ modulation).
Please also note that in resonance conditions the imaginary component becomes dominant and reaches the peak values, whereas the real component vanishes (resonant response is in fact ~90° out of phase with respect to the real, 0° excitation).
Lets e.g. collect the displacement in $z$ direction of the node at the center of the excited wheel contact area:
enter the POSTPROCESSING RESULTS menu, with opened t16 result file, and proceed within the HISTORY PLOT submenu
define the locations for the response sampling with SET LOCATIONS, hence click on the desired node[s], and finalize with END LIST
define the range of the sub-increments to be collected with INC RANGE, and then entering at the prompt 0:1 [enter], 0:397 [enter], 1 [enter], as the sampling beginning, end and step.
proceed with the definition of collected response diagrams by entering th ADD CURVES menu, and thenALL LOCATIONS (a single location has been selected); select the Frequency global variable as the abscissa, and the Displacement Z Magnitude nodal variable as the ordinate. The FIT scales the axes to contain all the sample points.
By hitting RETURN I may return to the HISTORY PLOT menu, where the label density may be reduced SHOW IDS from '1' to '10'; by entering a '0' value labels are hidden.
response peaks are now finite (they were theoretically unbounded in the absence of damping), and peaks disappear in correspondence of natural modes that are weakly coupled with the exciting force. In the absence of damping, bounded response at resonance is obtained for strictly uncoupled natural modes only.
Exam turn schedules
