mentat2013.1 -ogl -glflush  

====== Damped harmonic response ======

{{ :wikifemfuchde2019:monocoque_chassis_2019_v008.mud |}}

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 hit''OK'' 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 with''OK''
  * 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 then''ALL 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. 


====== Euler column buckling ======

base model: {{ :wikifemfuchde2019:400mm_supported_bar.mfd |}}

buckling load evaluation: {{ :wikifemfuchde2019:400mm_supported_bar.wxmx |}}

model at the end of today's lesson:{{ :wikifemfuchde2019:400mm_supported_barv002.mfd |}}

====== Flexural-torsional buckling example ======

{{ :wikifemfuchde2019:simplisupportedprofile_v000.mud |}}

profile made in s235jr steel

thickness:
{{tablelayout?rowsHeaderSource=Auto}}
^                            ^ thickness  ^
| flanges                    | 4 mm       |
| web                        | 2mm        |
| gusset plates at supports  | 4 mm       |

simply supported at gusset plate - lower flange intersection nodes (''support_me'' node set).


100kN load, uniformly distributed along the intersection line between the upper flange and the web spanning from support to supports (''load_me'' node set).
Please note that in MSC.Marc the supplied point load value is applied to **each** associated node.

Evaluate the peak equivalent von Mises stress along the structure according to the linear elastic modeling.

Due to the compressive state of the profile web, a check with respect to buckling is also required.

====== a few notes ======

{{ :wikipaom2017:schema_instabilita_v000.pdf |}}

====== Exam like exercises ======

===== Tubolar welded T-joint =====
The mesh elements are created along the midsurface
  * Aluminum (E=70000 MPa, nu=0.3, rho=2.7e-9 tonn/mm^3)
  * Chord:
    * average diameter: 50mm
    * wall thickness: 4mm
  * Brace:
    * average diameter: 40mm
    * wall thickness: 2mm

apply a torsional moment passing through the chord s.t. the nominal shear stress according to the beam theory is 1 MPa; evaluate the stress concentration at the joint as the peak equivalent von Mises stress (according to the employed discretization). 

{{ :wikifemfuchde2018:tubolar_section_properties.wxmx | nominal section properties}}

{{ :wikifemfuchde2018:t_joint_v000.mud |initial mesh}}

{{ :wikifemfuchde2018:t_joint_v006.mud |final version}}

===== Rollbar-like frame structure, o.o.plane transverse load =====

{{:wikifemfuchde2019:ooplane_loaded_frame.png?400|}}

{{ :wikifemfuchde2019:ooplane_loaded_frame.pdf |}}

Find the reaction force $V_\mathrm{A}$ and the reaction moments $\Phi_\mathrm{A}, \Psi_\mathrm{A}$ at the base of the directly loaded frame upright member; evaluate then the deflection $d$ at the load application point.

Numerically evaluate the unknown quantities with respect to the following dimensions
<code>
dim:	[
            a=800,
            b=1000, 
            E=210000,
            G=210000/2/(1+3/10),
            J=(40^4-36^4)*%pi/64,
            Kt=(40^4-36^4)*%pi/32
        ];
</code>

Solution: {{ :wikifemfuchde2019:outofplane_loaded_frame_v001.wxmx |}}

----