Front Impact Analysis using Hypermesh and RADIOSS
Problem Statement -
For the given reduced model of the front impact structure of a 4W automobile perform frontal crash analysis using hypermesh to setup the load case and RADIOSS as the solver.
Theory -
Any crash scenario involves huge changes in an object's inertia and leads to high dissipation of energy. This energy has to be absorbed by the car's structure before it reaches the passenger. This absorption of energy can only occur when the material deforms. Hence, the crash structure is designed in a way to crumple opposite to the direction of impact force and the remaining force is directed to the rest of the structure systematically.
The model given to us is restricted by the 100,000 nodes limit set by the hypermesh student edition. Mass of various parts such as the engine and drivetrain is added using the 'Add mass' feature. This ensures that although the model is reduced, it's center of gravity lies in the correct place, and the inertia of such heavy components is taken into account.
Procedure -
1.) Check unit system - This helps to avoid mistakes while inputting parameters to define the load case. Can be checked in the 'example_0000.rad' starter file.
2.) Create interfaces with recommended parameters - Interfaces are defined to model how parts interact when they come into contact with each other or themselves. For shell elements that have a thickness assigned, a gap/space is assumed between the master and the slave nodes. Spring elements with linear/non-linear stiffness are created between the slave nodes and their projections on the master elements. This is called the interface penalty method. The linearity of these assumed springs depends on the type of interface chosen. The type of interface depends on the nature of contact between the said parts.
a. Type 7 (variable stiffness) node to surface contact
b. Type 11 (variable stiffness) edge to edge contact
c. Type 19 (variable stiffness) Type 7 + 11
d. Type 24 (linear stiffness) node to surface and surface to surface contact
Important interface parameters that describe the nature of interface -
a. Igap - Determines how the size of the gap is calculated.
b. Gapmin - Minimum gap for activation of the interface.
c. Inacti - Action to take if initial penetrations exist.
d. Istf - Affects how the stiffness of the interface is calculated.
e. Iform - Friction formulation.
f. Stmin - Minimum stiffness to be used in the interface.
g. Idel - Deines what to do with the slave nodes and the master segments if the elements that they are attached to fails.
3.) Check for penetrations and intersections - Penetrations result if, in an interface, the slave node is closer to the master segment than the calculated gap. An error occurs in this case and the parameter - 'Inacti' offers options to remove any such penetrations. But before using any such automated methods, a penetration check and removal can be done manually.
4.) Create a rigid wall - A rigid wall does not physically exist but it is a kinematic condition imposed on the slave nodes. Rigid walls allow for an easy way to define an interface between a rigid surface and nodes of a deformable body. The rigid wall can be defined as - an infinite plane, a sphere, an infinite cylinder, or a parallelogram. The wall can be fixed or can have an initial velocity with respect to a local frame of reference.
5.) Add mass wherever necessary to achieve the target weight and center of gravity similar to a full car model -
For parts that don't contribute to the structure's stiffness but have a considerable mass that would affect the inertia and center of gravity of the car, masses can be added near their points of attachments. This can be done by creating groups of nodes or shells that demarcate the position of the part. Mass can either be added to each node/shell or can be distributed to each node/shell. This process has to be done for various parts of our car such as the engine & transmission, the fuel tank, rear seats, spare wheel, and doors. 
6.) Give an initial velocity to the vehicle - '/INIVEL ' define an initial velocity on a group of nodes. It does not require a function and does not vary with time. As require by the analysis, we provide an initial velocity of 35 mph or 15.6464 mm/ms.
7.) Create output requests for analysis of the crash -
a.) Sectional forces - To validate the flow of force from the front bumper rails to the A-pillar we create cross-sections of elements along this complete path and derive the normal forces acting on each section. Cross-section definition requires a local frame of reference and input of three nodes to further define the local skew. Also, a group of shells around the cross-section have to be input. This section can then be used as an input to a /TH (time history) output block which by default gives outputs of normal & tangential forces among many others. Similarily we create cross-sections at the front bumper rail, shotgun, A-pillar, and chassis front rail.
b.) Acceleration values at B-pillar - The aim is to output the deceleration values of the vehicle during the crash. This is achieved by placing an accelerometer sensor below the B-pillar since it does not undergo any deformation and would not have motion relative to the rest of the vehicle. This sensor once placed, has to be assigned a /TH output block to observe the values as time history plots. 
c.) Intrusion on the dash wall - The FMVSS 208 front impact test requires the intrusion value at the dash wall to be no more than 200mm. To validate this for our load case, we pick two nodes on the dash wall separated by some distance and connect them to the first crossbeam using a 1D 2 node spring element. The spring is assigned a very small mass and stiffness. The deformation of this spring with respect to its fixed point at the cross beam gives us the required output of intrusion. A /Th output block is assigned to obtain the deformations along Global X-axis among other outputs.
8.) Set stop time and time step for the animation and time history files
9.) Run the model checker - It checks for any and all potential issues that could terminate the solver when run. Issues such as incompatible kinematic conditions, under-defined or wrongly defined parameters, etc. can be corrected before running the simulation. We have no major errors after load case set up and only some insignificant warnings such as the presence of some free nodes that we created for reference. Such warnings can be ignored or dealt with using autocorrect tools.
Outputs and observations -
1.) Energy balance -
Total energy = Kinetic energy + Internal Energy - Contact Energy
2.) Cross-sectional forces -
Considering the hypothesis that the force travels from the bumper rails to the chassis rails and shotgun and finally to the A-pillars, our output graphs show a similar pattern. The most important parts of the crumple zone are the chassis rails and shotgun that have their highest strength during tensile and compression forces. This is validated by the output as the max force among all parts is at the chassis rail cross-section, 23.75kN followed by the shotgun, 11.5kN. The force tends to decrease as it reaches the A-pillar due to energy dissipation by parts in the crumple zone which is a desirable characteristic. Peak force at the A-pillar is 6.5kN which is the least among all parts. Hence we can validate the flow of force in our chassis.
3.) Accelerometer Reading -
Maximum deceleration of 325mm/ms2 occurs at the very start of the crash scene when the parts resist plastic deformation. It then sharply decreases as more and more energy is dissipated by the deformation of various parts. Short pulses of acceleration are due to the reaction forces that the parts exert in the strain hardening region before reaching complete plastic deformation.
4.) Value of intrusion at the dash wall -
FMVSS 208 requires the value of intrusion at the dash value to be not greater than 200mm. Our results suggest that we are well under that limit with a maximum intrusion of 45mm.
5.) Stress Contours -
The maximum value of von misses stress registered is 375N/mm2. Apart from that, the animation shows the direction and manner of deformation as predicted while designing the components. The passenger cabin shows almost low to no stress. With the addition of parts involved, a better understanding and accuracy of the solution can be obtained.
Learning Outcomes
1. Creating interfaces
2. Checking intersections and penetrations
3. Creating rigid walls
4. Mass balancing
5. Applying loading conditions
6. Obtaining potential warnings and errors using the model checker
7. Creating cross-sections and output requests
8. Setting up an accelerometer
Conclusion
The simulation shows to prove that a reduced model can provide close to accurate results which could save computation time and thus cost before design finalization. The longitudinal placement of rails to take advantage of their compressive strength and to direct loads to the rest of the chassis is validated by the simulation.
Google drive link -
https://drive.google.com/drive/folders/1chIlcl1w5-HtPg5Od_LchuD8pXk8J_Wo?usp=sharing