All Courses
All Courses
Courses by Software
Courses by Semester
Courses by Domain
Tool-focused Courses
Machine learning
POPULAR COURSES
Success Stories
QUESTION : Frontal crash-BIW Check unit system and either follow[Mg mm s] or [Kg mm ms]. Create appropriate interface ,friction 0.2 and recommended parameters. Make sure of no penetrations and intersection. Correct rigid bodies if any issues. Create rigid wall with friction 0.1. Compare the model weight with the full scale…
Sachin Barse
updated on 22 Aug 2022
QUESTION :
Frontal crash-BIW
OBJECTIVE :
CASE SETUP AND EXECUTION :
The given frontal crash vehicle model is as follows,
First, we will import the .rad starter file of the above model which is named as neon_front_0000.rad in Radioss using Import Solver Deck option. Then we will check the unit system which is followed in the model under BEGIN_CARD. So for this model, we will see that the unit system followed is [kg mm ms]. Now we will create all the required things for a frontal crash.
Penetration Check –
To check for penetrations in the model, we will go to Tools menu on Menu bar and click on Penetration Check option. In Penetration check panel, we will select all the components and click on Check command. The software will check for penetrations and then display the results as shown below,
So there are no penetrations or intersections in the model.
Interface –
For this model, we will create Type 7 interface for all the components of the model as it is self-impacting or the nodes and elements of the model will have a contact between them. We will go to Solver browser and we will delete all the existing interfaces. Then we will right click and navigate to Create > INTER > TYPE 7. Under Type 7 interface card, we will select all the components for slave nodes and master surface in Grnod_id(S) and Surf_id(M) respectively. Then we will define all the recommended parameters for Type 7 interface i.e. Istf = 4, Igap = 2, Idel = 2, Fscale_gap = 0.8, Stmin = 1 kN, Fric = 0.2, Gapmin = 0.5, Iform = 2. Here we will define Inacti as 0 which is default because there are no penetrations in the model.
Rigid Wall –
To create a plane rigid wall at the front side of the car, we will need the outermost node at the bumper of the car. So we will create the outermost node on the element edge using temp nodes option. Then we will right click in solver browser and navigate to Create > RWALL > PLANE.
For the location of rigid wall, we will click on the node which we created and then give a gap of 10 mm in X-axis as the wall must not be connected to the model. The normal of the wall will be in negative X-axis i.e. -1,0,0. Then we will specify the other parameters as follows.
The plane rigid wall will then be created.
Initial Velocity –
To create initial velocity, we will right click on Solver browser and then navigate to Create > BOUNDARY CONDITIONS > INIVEL. Under INIVEL card, we will select all the components as the Entity for grnd_ID. We will give the initial velocity of 35 mph or 15.6464 mm/ms in X-axis and as the velocity should be translational velocity, we will select TRA option in type.
Cross Section –
The results which we want on required cross sectional parts will be calculated based on a frame of reference. So before creating cross section, we will create moving frames on a particular node of that section. Now as we have to create the moving frames which are also called as local axis, we have to perfectly align our local axis to the global axis. So for this, we will extract the node location or coordinates of a particular node on the section in nodes panel. Then we will offset the node in X-axis by 10 units and create a new node. Similarly, we will offset and create a node in Y-axis as shown below.
Now we can create moving frame using these nodes. In Solver browser, we will right click and navigate to Create > FRAME > MOV. So here, we will create frame by node reference and select the nodes for x-axis and xy plane and then click on create.
Thus a moving frame will be created. Now we will create cross section for this frame. To create a cross section, we will right click on the Solver browser and navigate to Create > SECT > SECT. In section panel, we will specify the Frame_ID as the moving frame which we created and delta value as 0.1. From Hyperworks help menu, we get that the general value of alpha is taken as 2π102π10 . Thus we will specify alpha as 0.628. We will right click and create grshel_id, then we will select the elements where we want the cross sectional results.
Thus the cross section will be created as follows.
Similarly, we will create the cross sections at required parts namely A-pillar, Shotgun or Fender, Bracket and Rail. These cross sections will be created at both the sides i.e. left side and right side of the vehicle as shown below.
After creating the cross sections, we will request the results in TH or time history. For this we will go to Output Blocks under Model browser. Then we will right click and create a new output block. Under Entity IDs option, we will select the cross section which we created and thus we will be able to plot graphs of the cross sectional forces in HyperGraph.
In the same way, we will create the output blocks for the remaining cross sections.
Accelerometer –
We have to measure acceleration of B-pillar during the crash. So we will create accelerometers on both the B-pillars. To create accelerometer, we will right click in the Solver browser and navigate to Create > ACCEL. Then in node_ID, select the node on the B-pillar where we want acceleration result and specify F_cut value as 1.65.
The accelerometer will be created as follows.
Similarly, we will create another accelerometer on left B-pillar. Then we will create the output blocks for accelerometer in the same way as we did for the cross section to request time history results.
Intrusion –
Here, we need to find the intrusions on the dash wall at node 66695 and 66244 respectively. So to find the results at the specified nodes, we need to have a frame of reference. Thus we will create moving frames at Seat reinforcement part which is shown below.
Then, to obtain the results in HyperGraph, we will create output blocks for the intrusions by specifying the node and the frame or skew based on which the intrusions are calculated.
Mass Addition and Balancing (Required mass - 700 kg) –
At first, we will check mass and CG of the vehicle. For better visualization, we will use HyperCrash software to check mass and CG of the vehicle.
In the above figure, we can see that the mass of the vehicle is 188 kg and the CG of the vehicle is at the black circle. In general, the CG of the vehicle is somewhere just behind the driver’s seat. So in order to get the required CG location, we will do mass balancing by adding some on the panel where the passenger seats are located. We also have to get the mass of the vehicle to 700 kg. So in Hypermesh, under solver browser, we will right click and navigate to Create > ADMAS. In ADMAS panel, we will specify the required mass to selected nodes and for Mass type, we will select Mass/node option.
In this way, we will create Rear_Mass and Front_Mass and balance them to get 700 kg and Cg at required position. Since this model is not the complete vehicle model, the point of CG which will be obtained won’t represent real life scenario. Thus we will not concentrate much on the Z-axis of the CG point and we will get CG below the floor panel as shown below.
In the above figure, we can see the Total mass of the vehicle in red box as 700 kg.
Time Step and Run time –
To check these parameters in Hypermesh, we will navigate to Cards under Model browser. To check the run time, we will open ENG_RUN card where we will see that the model already have the run time in Tstop as 80 ms. For the time step, we will open ENG_DT_NODA card and we will change the Tmin value to 0.5 microseconds or 0.0005 ms.
Model Checker –
To check the quality of the model in Hypermesh, in Menu Bar we will navigate to Tools > Model Checker > RadiossBlock. This will open a new Model Checker browser.
In this browser, we will click on Run checks command which is at the top right side in the above figure, indicated in red box. After running the checks, we will click on Auto correct command which is in blue box, through which the software will automatically perform the possible corrections and give a green tick in status bar. From above figure, we can ensure that the quality of the model is good for simulation. The error which says the nodes N1, N2, N3 badly defined, can be ignored as the sections are assigned to moving frames which are created separately. Other errors and warnings can also be ignored.
Now we can proceed to run the simulation. So we will navigate to Radioss in Analysis page. Here we will save the model to a specified path and in options, we will type –nt 4 and then click on Radioss option to run the analysis.
SIMULATION AND RESULTS :
First, we will check Energy error and Mass error. So we will open the engine .out file of the model and check the last column for Energy and Mass error as shown below.
The red box indicates Energy error which is -2.2% and blue box indicates Mass error which is very negligible. This shows that the energy error and mass error are within acceptable range.
The total number of cycles used is 160001 and the total runtime of the simulation is 4820.95 s.
To view the simulation results, we will switch to HyperGraph. In HyperGraph, we will load .h3d file from specified path and we will play the simulation.
In the above crash simulation of the vehicle, we can see the vehicle body is impacting on the rigid wall. After the impact, the frame of the vehicle deforms and the vehicle has a pitching movement about its CG point. As this model is a reduced model and not a complete model, the deformation is unrealistic.
From the Von Mises stress plot, we can say that the stress distribution is quite good in the vehicle after the crash. There are very few areas where we can see stress concentration. Generally the stress is more in bumper region as it is the first point of impact.
Energies –
From the above plot, we can see that there is high amount of Kinetic energy at the start of the simulation but as the simulation progresses, the kinetic energy in the vehicle decreases and gets converted into internal energy, so the internal energy increases in the same proportion. Thus the total energy in the system is almost constant at 85000 J and due to some energy loss which we can see in energy error, there is some decrease in total energy. We can also see some amount of contact energy in the model as we have defined the value of friction in Type 7 interface due to which contact energy is generated.
Cross Sectional Forces –
From the above plot, we can see that the resultant forces experienced on the right A-pillar is more than that experienced on the left A-pillar.
From the above plot, we can see that initially the resultant forces experienced on the right side Shotgun was higher but as the simulation progresses, the forces at left side Shotgun is much more than that experienced on the right side Shotgun.
From the above plot, we can see that the resultant forces experienced on the right Bracket is more than that experienced on the left Bracket.
From the above plot, we can see that initially the resultant forces experienced on the left side of the Rail was higher but as the simulation progresses, the forces at right side of the Rail is much more than that experienced on the left side of the Rail.
Accelerometer –
Initially, the acceleration of the right B-pillar was higher but as the simulation progresses, the acceleration of the left B-pillar is more or somewhat similar to right B-pillar. The maximum acceleration of right B-pillar is 3 m/s2 whereas the maximum acceleration of left B-pillar is 2 m/s2.
Intrusions –
The resultant displacement at node 66244 is 900 mm and the distance between the node 66244 and node of its respective skew is 793.73 mm. Thus the intrusion at node with ID 66244 is 900 – 793.73 = 106.27 mm. Similarly the distance between the node ID 662695 and node of its respective skew is 767.62 mm and the resulting intrusion is 900 – 767.62 = 132.38 mm.
CONCLUSION :-
The vehicle model is impacted on a rigid wall to study the frontal crash scenario of the vehicle. As the model is reduced to limited parts, we get unrealistic deformations and results. Thus the center of gravity of the vehicle along with vehicle mass is very important and it mainly decides the behavior of the vehicle under crash.
Leave a comment
Thanks for choosing to leave a comment. Please keep in mind that all the comments are moderated as per our comment policy, and your email will not be published for privacy reasons. Please leave a personal & meaningful conversation.
Other comments...
FINAL INDEPENDENT PROJECT
Project : Design & Animate the drone camera for project model. Attached Link For Model Review : https://drive.google.com/file/d/1f6sjaJc6Od2AEnmh-JYFFoLMmUveWk61/view?usp=drive_link
15 May 2024 05:42 PM IST
Week - 4
AIM: Implement control logic of a “washing machine” using Stateflow as per given sequence: If the power supply is available, the system gets activated. If the Water supply is not available, stop the process & indicate through LED Soaking time should be 200s followed by Washing…
13 Mar 2024 10:27 AM IST
Week -2
1.Door Bell Simulink Model: Simulink Model Explanation: The pulse generator is used to create square wave pulses at regular intervals.The block waveform parameters Amplitude,pulse width,period and phase delay,determine the shape of the output waveform. …
12 Mar 2024 12:23 PM IST
Project 1
Attached Model for Project :- Attached link for grading :- https://drive.google.com/file/d/13bjiEKi2h1sYtm9LzZMouMksFAZYnVIQ/view?usp=drive_link
29 Oct 2023 11:00 AM IST
Related Courses
Skill-Lync offers industry relevant advanced engineering courses for engineering students by partnering with industry experts.
© 2024 Skill-Lync Inc. All Rights Reserved.