Side Pole Crash Simulation Challenge | HyperMesh

OBJECTIVE :

• To perform side crash analysis of a vehicle against a rigid cylindrical wall or a Pole in Hypermesh.
• To simulate the crash behavior of the vehicle in HyperView and discuss the results.
• To plot the sectional forces at cross members and discuss the results.
• To obtain intrusion results at B-pillar, hinge pillar and fuel tank region and plot them in HyperGraph.
• To obtain peak velocity of inner node of the door.

CASE SETUP AND EXECUTION :

The given side crash vehicle model is as follows,

First, we will import the .rad starter file of the above model which is named as neon_side_reduced_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 side 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 (Pole) –

To create a cylindrical rigid wall at the left side of the car, we will need the outermost node at the front left door 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 > CYL. In the RWALL panel, under Engineering data we will specify the coordinates of the pole which will be at some distance from the outermost node on side door. Then we will give the normal direction to the pole in Z-axis and diameter of the pole to be 254 mm. The FRIC value will be 0.1 and Dsearch value will be 1000 as shown below.

The cylindrical rigid wall or the Pole will then be created as shown below.

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 Y-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 `(2π)/10` . 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 both the cross members 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.

Intrusion –

Here, we need to find the intrusions at B-pillar, hinge pillar and fuel tank. So to find the results at the specified parts, we need to have a frame of reference. Thus we will create moving frames at the opposite side i.e. at right B-pillar, hinge pillar and fuel tank of the vehicle as 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.

Peak velocity of inner node of the door –

To find peak velocity at the inner node of the door, we will create a moving frame at the node location by using the same procedure as we used in cross section creation. Then we will create output block for the peak velocity by specifying the node and the frame or skew based on which the peak velocity is calculated as shown below.

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 166 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 mass on the cross members and on the rails. 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 balance the mass 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 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 row for Energy and Mass error as shown below.

The red box indicates Energy error which is -3.1% 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 7590.47 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 a Pole. After the impact, the frame of the vehicle deforms and the vehicle body gets contracted around the pole with left B-Pillar as the pivot point. The CG of the vehicle is in the same axis or direction of the pole, so we can see even deformation of the frame around the pole.

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 B-pillar and cross members as B-pillar takes the initial impact and then the impact is transferred to the cross members.

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.

Sectional Forces in Cross Members –

From the above plot, we can see that the total resultant force in the rear cross member is more than the front cross member. As the rear cross member is in line with the Pole, it experiences more force.

Intrusions –

Intrusion at Fuel Tank – The final displacement at fuel tank region is 1515.37 mm and the initial distance of fuel tank from frame of reference is 1319.71. So total intrusion is 1319.71 - 1515.37 = -195.66 mm. Thus the total intrusion at fuel tank region is 195.66 mm but the minus sign indicates that the intrusion is increased after the crash. This increase of intrusion can lead to failure of fuel tank and fuel may drop out of the tank. To prevent this failure, we need to reduce the intrusion which we can achieve by adding another cross member in fuel tank region which absorb some energy and resist the movement of fuel tank region and also the cross member can take some deformation.

Intrusion at Hinge Pillar – The final displacement at Hinge Pillar region is 1366.50 mm and the initial distance of fuel tank from frame of reference is 1312.65. So total intrusion is 1312.65 - 1366.50 = -53.85 mm. Thus the total intrusion at hinge pillar region is 53.85 mm but the minus sign indicates that the intrusion is increased after the crash.

Intrusion at B-Pillar – The final displacement at Hinge Pillar region is 1428.05 mm and the initial distance of fuel tank from frame of reference is 1317.25. So total intrusion is 1317.25 - 1428.05 = -110.8 mm. Thus the total intrusion at hinge pillar region is 110.8 mm but the minus sign indicates that the intrusion is increased after the crash.

Peak Velocity –

The inner node of the door experiences resultant velocity as shown above. The Peak Velocity is of 15.6464 m/s at the start of the simulation as we have given the exact same value of initial velocity to all the components in INIVEL card. After the pole impact, there is no velocity on the door because the motion of the door comes to a halt near the pole.

CONCLUSION :

The vehicle model is impacted on a rigid Pole to study the side crash scenario of the vehicle. As the model is reduced to limited parts, we get somewhat 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.