Week - 5 - Modelling Spotwelds

AIM : To model spotwelds for the given assembly of parts and run a crash test in LS-DYNA.

OBJECTIVES:

• To create a rigidwall in LS-Dyna on which the spotweld model can impact.
• To apply initial velocity of 50 kmph to the model.
• To run the simulation of model using two different types of spotweld i.e. beam spotweld and solid element spotweld.
• To plot the cross-sectional force generated in the middle of the model.
• To plot and compare the forces and results for both the type of spotwelds.

CASE SETUP:

Spotweld is used to connect multiple or overlapping pieces of metal. To analyze the strength and failure of the spotweld at connection points, we will simulate its behaviour with a crash test. The given model for spotweld is as follows.

     

For this model, we have to connect the top surface and the bottom surface with spotweld. So, the spotwelds will be modeled by using 1D beam elements and solid elements. The 1D beam elements will be created in Element Generation panel by using Two Node Sets and solid elements will be created in Element Editing panel by using Hexa elements. The resulting 1D beam and solid beam elements connecting both the surfaces are shown below.

     

Rigidwall –

To create a planar rigidwall at one of the sides of the model, we will follow the procedure mentioned below.

• Go to Create Entity
• Under Rigidwall sub panel, go to Cre to create a new rigidwall.
• Select Planar option and under GeoVector select 1n+NL
• Select one of the nodes on the edge of the model. The rigidwall will then be created on the edges of the model so we will translate it by some distance so as to have space between the rigidwall and the model.
• Under GeoVector, select Trans option and translate the rigidwall by 15 mm in X-axis. The rigidwall will be created as shown below.

     

Initial Velocity –

The initial velocity of 50 kmph must be applied to the model in order to give translational motion to the model for impact with the rigidwall. So before creating the initial velocity keyword, we will create node set for all the shell elements of the model.

• Go to Create Entity
• Under Set Data sub panel, go to Cre to create a new *SET_NODE by selecting all the elements of the model.

Thus the node set for model is created. Now we will create Initial velocity keyword to impose velocity to the elements of the model.

• Go to Keyword Manager
• Select INITIAL > VELOCITY card and mention the node set ID which was created earlier.
• As we have to use gm-mm-ms unit system, we will provide initial velocity of 89 mm/ms (i.e. 50 kmph) in x-direction.

Material –

For the model, we will assign the material as steel which is a non-linear characteristic material.

• Go to Keyword Manager
• Select MAT > 024-PIECEWISE_LINEAR_PLASTICITY material card. Give it a material ID and title.
• As we are using gm-mm-ms unit system, we will provide the characteristic values of steel as follows.
  • Density of Steel (RO) – 8.05 x 10^-3 gm/mm³
  • Young’s Modulus (E) – 210 x 10³ MPa
  • Poisson’s Ratio (PR) – 0.3
  • Yield Stress (SIGY) – 250 MPa
  • Tangent Modulus (ETAN) – 1000 MPa

     

Now, for both the type of spotwelds, i.e. 1D beam spotweld and solid spotweld, we will use MAT_100/*MAT_SPOTWELD. Here we will provide the same characteristics of steel as provided earlier. For time based failure, we want our spotweld to fail at 2.5 ms. The effective plastic strain will be 10% and other parameters will be as follows.

     

Thus the material card is ready as shown above.

Section –

Section card is required to define section properties for 1D beam and solid beam elements. For all the shell elements, we will define *SECTION_SHELL card with element formulation ELEFORM as 16 and the thickness of shell elements will be 1.5 mm.

     

Now we will define section for beam and solid element respectively. Since we used material type 100, the material model will only apply to beam element type 9 and to solid element type 1. Thus for *SECTION_BEAM, we will define ELEFORM 9 and for *SECTION_SOLID, we will define ELEFORM 1 respectively as shown below.

     

     

Hourglass –

We will Define hourglass and bulk viscosity properties which are referenced using HGID in the *PART command. This keyword will control the hourglass energy which can be generated in the elements which produce no strain or stress.

• Go to Keyword Manager
• Select HOURGLASS Give it an hourglass ID and title.
• Select Hourglass control type (IHQ) as 2 and keep rest of the values as default.

Now we will define all the corresponding characteristics to the Top surface, Bottom surface and Spotweld part in PART keyword respectively.

Contact –

We will have to define contact between the spotweld elements and top and bottom surface, as well as a self-contact for the model as the elements may have a contact between themselves after the deformation. So for self-contact, we will define AUTOMATIC_SINGLE_SURFACE contact with coefficient of friction 0.2 as shown below.

     

For the model having 1D beam elements, we will define *CONTACT_TIED_SHELL_EDGE_TO_SURFACE as it contains 1D element. The slave nodes will be the nodes containing spotweld elements whereas the master part will be the top and the bottom part of the model. The other parameters will be default as shown below.

     

For the model having Solid beam elements, we will define *CONTACT_SPOTWELD as it contains spotweld hexa elements. Similarly, the slave nodes will be the nodes containing spotweld elements whereas the master part will be the top and the bottom part of the model. The other parameters will be default as shown below.

     

Control –

We will define the termination time of the simulation which is necessary to run the simulation. Thus we will define the termination time as 5 ms in CONTROL SIMULATION Keyword. We will also define CONTROL_ENERGY card to provide controls for energy dissipation options.

Database –

We have to find cross sectional forces generated in the middle of the model, so will create a cross section at the middle.

Cross-Section –

• Go to Create Entity
• Under Database sub panel, select Cross Section and go to Cre to create a new cross-section.
• Select the node and the axis where the cross section plane must be located and then click on Apply. The cross-section will be created as follows.

     

History node –

We will create a node history database card as we want the acceleration plot at a node in the middle portion of the model. So, in this card we will select one of the center node (501571) of the model in the node ID option.

History Beam and History Solid –

To obtain the plot of axial forces, shear forces and other necessary forces on the 1D beam element as well as solid beam element, we will create History_Beam Keyword and History_Solid Keyword for 1D beam and solid beam element respectively as shown below.

     

     

Binary Plot –

After defining all the conditions required for simulation, we can generate output requests or results which we are interested in the model. So we will define BINARY_D3PLOT under DATABASE keyword and specify Time interval between outputs DT as 0.1 ms.

In Database ASCII, we will ask for GLSTAT, MATSUM, NODOUT, RCFORC, RWFORC, SECFORC, SLEOUT, SWFORC, etc each with DT as 0.1 ms.

Now we will check our model with the Model Check command in Keyword Manager. If there are no errors in the model, then we can proceed for the simulation.

After creating all the necessary files for simulation and checking the model, we will save the model as Keyword file with .K extension. To run the model, we will go to File > Run LS-DYNA. We will browse this keyword file and then run the simulation for 1D Beam element and then for Solid Beam element.

In this case, the simulation ended with Normal Termination so both the model was successfully simulated.

RESULTS AND PLOTS:

To run the simulation, we will open the binary d3plot file form specified path. Then we will click on Play button on Animation Toolbar. The resulting animation is shown below.

Results of 1D Beam Model –

     

     

Based on the above simulation, we can say that the Spotweld breaks or fails after time 2.5 ms, exactly as we have defined. The bottom surface of the model impacts the rigid wall and due to the momentum, the top surface is in motion which is resisted or held by the 1D beam elements until they fail. The kinetic energy of the bottom surface is transferred to rigidwall or converted to internal energy, so after the impact the rebound velocity reduces.         

Von-Misses Stress –

     

In the above animation, we can see that after the impact, there are stresses developed throughout the model. Initially, the stress concentration is maximum at the impact region near the rigid wall and then the stress concentration can be seen at all the spotweld regions. The stress distribution is uneven due to the vibrations induced in the model after the impact as the simulation progresses.

Energies Plot –

     

In the Energies plot, we can see that the kinetic energy of the model decreases after the impact at 1 ms and it gets converted to internal energy in the model. Thus the Total Energy of the system is constant. The hourglass energy generated in the model is almost negligible. At 1.2 ms, the nature of the graph slightly changes as the top surface of the model experiences some resistance to the movement due to the spotweld.

Cross-Section Force –

     

The plot of resultant force with time is along the length of the model where we located the cross-section plane. The maximum force of 28.5 kN is experienced at 1.2 ms after the impact.

Nodal Acceleration –

     

As the model is moving and impacting in X-axis, we will plot the X-acceleration of Node 501571. The maximum value of the acceleration at Node ID 501571 is seen at 3.9 ms. After the impact, the model goes into vibration and thus we can see the acceleration plot in positive as well as in negative X-axis.

X Stress –

     

The stresses generated on the model in X-axis are shown above. The maximum stress generated on X-axis is 371.225 MPa at element ID 107998 which is one of the element on bottom surface connecting beam element.

Y Stress –

     

The stresses generated on the model in Y-axis are shown above. The maximum stress generated on Y-axis is 288.367 MPa at element ID 106900 which is at the edge of the bottom surface and near the rigid wall.

Effective Plastic Strain –

     

From the above shown Effective Plastic strain animation, we can see the maximum strain at the spotweld region.

Spotweld Axial Forces –

     

The axial forces of all the beam elements are somewhat similar. As it is a 1D beam element, it will experience more axial force than shear force. Here the maximum axial force is 1.8 kN at 2 ms and then axial forces becomes zero when the beam element breaks at 2.5 ms.

Spotweld Shear Forces –

     

Here also the shear forces of all the beam elements are somewhat similar. As it is a 1D beam element, it will experience less shear force than axial force. The maximum shear force experienced by one of the element is 760 N at 1.35 ms.

Results of Solid Beam Model –

     

     

Based on the above simulation, we can say that the Spotweld breaks or fails after time 2.5 ms, exactly as we have defined. The simulation is somewhat similar to 1D Beam model simulation. The bottom surface of the model impacts the rigid wall and due to the momentum, the top surface is in motion which is resisted or held by the solid beam elements until they fail. Also the kinetic energy of the bottom surface is transferred to rigidwall or converted to internal energy, so after the impact the rebound velocity reduces. 

Von-Misses Stress –

     

Here also, we can see that after the impact, there are stresses developed throughout the model. Initially, the stress concentration is maximum at the impact region near the rigid wall and then the stress concentration can be seen at all the spotweld regions. Comparing 1D Beam model, the magnitude of stress generated in this model is less.

Energies Plot –

     

Comparing this energy plot to the 1D beam plot, we can see that the total energy of the both the plots are same. The reduction in kinetic energy is more in this plot as the solid spotweld element increases the mass of the model and thus decreases kinetic energy after impact. The nature of the graph at time 1.2 ms, when it experiences some resistance in motion due to spotweld is smooth comparatively.

Cross-Section Force –

     

The forces experienced on the cross section plane of the model are more in magnitude compared to forces experienced on the beam model. The maximum force experienced is around 32 kN whereas in beam, it is around 28.5 kN.

Nodal Acceleration –

     

Comparing the acceleration plot with the Beam model’s acceleration plot, we can see that the acceleration of the solid element model in X-axis is higher than beam element model after the impact. Here also the model goes into vibration and thus we can see the acceleration plot in positive as well as in negative X-axis.

X Stress –

     

The stresses generated on the model in X-axis are shown above. The maximum stress generated on X-axis is 326.78 MPa at element ID 109580 which is one of the element on bottom surface connecting solid spotweld element.

Y Stress –

     

The stresses generated on the model in Y-axis are shown above. The maximum stress generated on Y-axis is 273.362 MPa at element ID 108578 which is one of the element on bottom surface connecting solid spotweld element.

Effective Plastic Strain –

     

From the above shown Effective Plastic strain animation, we can see the maximum strain at the spotweld region.

Spotweld Axial Forces –

     

The axial forces of the solid elements of top faces and elements of side faces are different. As it is a solid spotweld element, it will experience less axial force than shear force. Here the maximum axial force is 475 N at 2 ms and then axial forces becomes zero when the beam element breaks at 2.5 ms.

Spotweld Shear Forces –

     

Here the shear forces of all the solid spotweld elements are somewhat similar. As it is a solid element, it will experience more shear force than axial force. The maximum shear force experienced by one of the element is 1.8 kN at 1.35 ms.

CONCLUSION:

The crash test of the model having spotweld connections is simulated. By comparing all the results and simulation for two different types of spotwelds, we can say that there is some change in results and plots as discussed above. Thus, we can conclude that change in type of spotweld will affect the results and simulation behaviour of the model.