Strumenti Utente

Strumenti Sito


Initial model


Step by step evolution: v001 v002 v003 v004 v005

v005b, with the added sway bar linkage.

Inertia relief model, without added masses v007, and with the added masses v008 v009.

Front impact, with or without ground support v010 v011 v012.

Dynamic modal loadcase v013 v014 v015 v016


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.

Thinner panels: 1.8mm aluminum sheet, 6.75mm 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





The pedagogical model proposed does not include sway/antiroll bars, that are instead a critical element for torsional stiffness loadcases.

In particular, torsional stiffness should be evaluated in both the limiting cases of

  • rigid springs, disconnected sway bars;
  • disconnected springs, rigid sway bar.

This second loadcase, which is usually neglected, is however relevant for sizing the sway bar support areas on the chassis structure.

On the relevance of constraining in dynamic analyses. back view side view relevance of (improper) constraints on the dynamic behaviour of a structure. Design is reliable in actual operational conditions (link). Added constraints stiffen up the structure, thus increasing natural frequencies. However, a 0 Hz rigid body mode natural frequency may rise to a finite value due to added positioning constraints; the associate natural mode may be excited in resonance by dynamic loads.

How to set a damped response

Click here to expand

Click here to expand

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:

  • preemptively define a modulating table 1/ω
    • define NAME as modulate_stiffmatmult
    • set Indipendent variable v1 TYPE as frequency
    • define table through FORMULA and type 1/pi/v1, i.e. $g(f)=\frac{1}{\pi f}$
  • 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.


Poor man dynamic response animated view

MSC.Mentat procedure for creating poor man harmonic response animations

MSC.Mentat procedure for creating poor man natural mode animations

Structural damping references





estratto vol. 2, sezione 8 di Soovere, J., and M. L. Drake. Aerospace Structures Technology Damping Design Guide.LOCKHEED-CALIFORNIA CO BURBANK, 1985.


  • Static test: torsional stiffness;
  • Front, right wheel bump loadcase (inertia relief);
  • 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).
  • Dynamic modal response;
  • Dynamic harmonic response: vertical harmonic load at the front, right wheel, 1-100 Hz range, sampled at 0.25Hz resolution ((100-1)*4+1 = 397 steps);


wikifemfuchde2020/phoneyfsaechassis.txt · Ultima modifica: 2020/05/28 16:40 da ebertocchi