Modelling Spotwelds in LS Dyna

OBJECTIVE: 

1. To model a set of spot welds for the given assembly of parts by using both 1d beam elements and 3d Hexa elements. 
2. To simulate a crash test for the given assembly and compare the results in both the cases.

   • Deliverables ==>

     - Input .k file and output files (d3plot, glstat, sleout, rcforc) - Animation of the final simulation - The cross-sectional force generated in the middle of the crash box (along its length) - Acceleration plot of a node  in the middle of the crash box (along its length) - Maximum directional stress and strain along the length of the crash box (X strain, Y strain, etc) - A plot of all energies (total, internal, kinetic, hourglass, sliding) - Compare the results

PROCEDURE:

1. Solver-deck set-up
   1. Open the given FE model in LSPP(LS-PrePost). The model consists of 2 parts. Note: We need to define all the attributes related to the parts as well as create a set of spot welds to connect the two parts. This has to done in two ways, first by modeling the welds using 1d beam elements and second, by using 3d Hexa elements. Both the models will then be subjected to a crash test and the results are to be compared.

      Fig. 1. The imported keyword file

   2. Create and assign appropriate material and section cards to the two parts. Note: Here properties of steel are used for defining the material card.

      Fig. 2. The material and section cards assigned to the two parts

   3. Now we need to connect the two parts using spot welds. Here, we will model 8 spot welds in a symmetric manner, i.e, 4 on each side. Create beam elements using the EleGen option under the Mesh button.

      Fig. 3. Beam elements(8nos) created to model the spot welds

   4. Now we have to create and assign material and section cards for the created beam elements. *MAT_SPOTWELD card is used for defining the material for the spot weld beam and *SECTION_BEAM card is used for defing the section for the beam elements. All the beams are included in PID 100. In order for the welds to fail midway the simulation, we will set the TFAIL value as 2.5 ms(as we intend to run the simulation for 10 ms).

      Fig. 4. Material and section cards for the beams representing the spot welds.

   5. Now we need to define appropriate contacts for the assembly. To define the contact between the beam elements and the two joining parts, we can use the *CONTACT_TIED_SHELL_EDGE_TO_SURFACE card, keeping the beam elements as the slave and the two brackets as the master segment. Another contact, *CONTACT_AUTOMATIC_SINGLE_SURFACE has to be created for defining the interaction between the brackets during the crash.

      Fig. 5. Contact cards defined for the crash

   6. Now we need to create a rigid wall and apply an initial velocity to the assembly of parts for simulating the event of a crash. The *RIGIDWALL_PLANAR card is used to define the rigid wall. The wall is created 10 mm away from the bracket. *INITIAL_VELOCITY card is used to assign an initial velocity of 10mm/ms in the global X direction.

      Fig. 6. A rigid wall created and initial velocity applied to the parts

   7. We need the simulation to run for 5 ms. This can be defined using the *CONTROL_TERMINATION card and assigning the DT value as 5.

      Fig. 7. Setting the simulation runtime using the *CONTROL_TERMINATION card

   8. Now the solver deck has been set up for the 1st case. In the 2nd case, we need to model the spot welds as Hexa elements or solid elements. We will use the already created 1st case solver deck and modify it to set the solver deck for case 2. We will first delete all the beam elements and replace them using solids Hexa elements. The Hexa elements are created using the element creation option under the EleTool button. After creating the Hexa elements, we can make use of the already existing material cards to assign the material for the solids. Now delete the section created for beam and create a new solid section with element formulation 1 and assign it to the solids created. The contacts also need to be changed fro case 2. This time, we will use the *CONTACT_SPOTWELD card to define the spotweld connection using the Hexa elements. Rest everything can be kept as same for both the cases.

      (i)	(ii)
      Fig. 8(i) Case 1(Using 1d beam elements); (ii) Case 2(Using 3d Hexa elements)

2. Output request
   1. We have to create appropriate database cards to request for particular results.
   2. Use *DATABASE_ASCII_option card to request for glstat, matsum, sleout, rcforc, rwforce, swforc, nodout, and secforc. The glstat will record all the global energy values throughout the simulation. The swforc will record the values related to the Spot weld. The rwforc will record the forces recorded on the rigid wall. The secforce and nodout will record the values associated with a particular section and node defined using the cards *DATABASE_CROSS_SECTION_PLANE_ID and *DATABASE_HISTORY_NODE respectively.

      Fig. 9. Output requests made using the ASCII card

   3. Define *DATABASE_CROSS_SECTION_PLANE_ID and *DATABASE_HISTORY_NODE cards for section and node respectively.

      Fig. 10. The *DATABASE_CROSS_SECTION_PLANE_ID and *DATABASE_HISTORY_NODE cards

   4. Create *DATABASE_BINARY_D3PLOT to record the animation for the simulations.

      Fig. 11. The *DATABASE_BINARY_D3PLOT card

   5. Make the same output requests for both the cases.
   6. Now we have completed the entire solver deck along with output requests and our Keyword files fro both the cases are ready for analysis. Open the launch manager and run both the keyword files.

RESULTS & DISCUSSION: 

1. Crash animation

   (i) Case 1	(ii) Case 2
   Fig. 12. Crash animation
   The crash animation shows the assembly crashing against the rigid wall at ~ 1 ms. All the spot welds fail at exactly 2.5 ms in both cases.  In both cases, on impact against the wall, the bottom bracket tends to bounce back. This rebound motion of the bottom bracket is transferred to the top bracket via the spot welds. After the failure of the spot welds at 2.5 ms, the top bracket is no longer restrained by the bottom bracket and begins to freely move ahead with its inertia. While in case 1, the bottom bracket can be seen to have come to nearly zero rebound velocity due to the inertia effect of the top bracket, in case 2, the assembly appears to be stiffer and there is almost zero rebound, possibly due to higher inertia of the whole assembly arising from the use of solid elements to represent the welds.

2. Stress contour

   (i) Case 1	(ii) Case 2
   Fig. 13. Stress contour
   Stress contour shows the stresses getting developed on the two brackets as the crash takes place.  A greater amount of stress seems to have transferred to the top bracket in case 2. Red regions signifying stress concentration are present near the spot weld regions in case 2. This may be because of a greater stiffness value for the spot welds modeled using solid elements.

3. Plastic strain contour

   (i) Case 1	(ii) Case 2
   Fig. 14. Plastic strain contour
   The maximum strain recorded were 0.00384 and 0.0047 for case 1 and 2 respectively. The region around the spot welds can be seen to have gotten strained in case 2 whereas nothing like that is observed in case 1.

4. Stress-strain plots

   (i) Case 1	(ii) Case 2
   Fig. 15. Stress-strain plots
   The figure shows the stress-strain plot generated by using the stress and strain values recorded on element number 106880. The stress-strain plots for both cases are identical. The material defined for the model has a yield stress of 250 MPa. Here, the maximum stresses observed are 136 MPa and 167 MPa for cases 1 and 2 respectively.

5. Stress plots

   (i) Case 1	(ii) Case 2
   Fig. 16. Stress plots
   The stresses recorded of element number 106880 was plotted against run time to obtain the stress plots shown in the above figure. The plots show a higher amount of stress being recorded in case 2 compared to case 1.  The maximum stresses are 137 MPa and 167 MPa for cases 1 and 2 respectively.

6. Strain plots

   (i) Case 1	(ii) Case 2
   Fig. 17. Strain plots
   The strain plots were also generated from the values recorded for element number 106880.  The two plots are very identical with not much difference.

7. Global energy plots

   (i) Case 1	(ii) Case 2
   Fig. 18. Global energy plots
   The global energy plots are as expected. The total energy remained constant throughout the simulation while the kinetic and internal energies kept on changing as the crash happened. Kinetic energy can be seen decreasing at ~ 1ms when the impact takes place. This decrease in Kinetic energy is reflected as a corresponding increase in Internal energy. The Internal energy reaches a peak when the bottom bracket is at the verge of rebounding and it then decreases as the bracket rebounds with some velocity. Again due to the inertia factor of the top bracket, this rebound velocity decreases, which explains the increase in the internal energy at ~1.2 ms before finally coming to a constant value close to 80 N-m in case 1. This value is much higher(92 N-m) for case 2.

8. Acceleration plots

   (i) Case 1	(ii) Case 2
   Fig. 19. Acceleration plots
   The acceleration plots were generated from the history data of node number 508406 in both cases. The plots are identical. The Max acceleration recorded is 1600 `(mm)/(ms)^2` and 1510 `(mm)/(ms)^2` for cases 1 and 2 respectively.

9. Velocity plots

   (i) Case 1	(ii) Case 2
   Fig. 20. Velocity plots
   The velocity plot shows a uniform velocity of 10 `(mm)/(ms)` until the impact and thereafter, the velocity decreases and goes to a negative value and finally becomes nearly zero as the simulation progresses. However, in case 2, after rebounding, the bracket has again achieved a positive velocity owing to a higher inertia factor in this case.

10. Sectional forces plot

    (i) Case 1	(ii) Case 2
    Fig. 21. Sectional forces plot
    The above plot shows the resultant force recorded on a section created on the top bracket just after the weld regions. The graphs show that a higher amount of force has been transferred to the top bracket in case 2. The max force recorded in case 2 is 14200 N whereas the same recorded for case 1 is only 3130 N. This can be a result of the Hexa elements being used to model spot welds in case 2.

11. Spot weld Resultant forces

    (i) Case 1	(ii) Case 2
    Fig. 22. Spot weld Resultant forces
    The max resultant force for case 1 is 466 N and for case 2 is 1950 N.

12. Spot weld axial force

    (i) Case 1	(ii) Case 2
    Fig. 23. Spot weld axial force
    Axial forces recorded for case 2 are significantly higher compared to the ones recorded for case 1. This further implies the increased stiffness in the case of Hexa elements.

13. Spot weld shear force

    (i) Case 1	(ii) Case 2
    Fig. 24. Spot weld shear force
    Shear forces on the weld elements in case 1 are significantly lower compared to the values for case 2. The max shear force recorded for case 1 is 276 N whereas the same recorded in case 2 is 1890 N.

14. Spot weld length

    (i) Case 1	(ii) Case 2
    Fig. 25. Spot weld length
    The spot welds modeled using 1d beam elements undergo elongation on the application of force, whereas the ones modeled using Hexa elements don't undergo any elongation. This is clearly observed from the above graph.

15. DIRECTIONAL STRESS AND STRAIN VALUE COMPARISON

    	Max-Stress(MPa)			Max-Strain
    Case	X-Direction	Y-Direction	Z-Direction	X-Direction	Y-Direction	Z-Direction
    1	267.2 on Ele 108672	218.9 on Ele 106963	189.9 on Ele 109915	0.00119 on Ele 108672	0.00105 on Ele 108321	0.00093 on Ele 109915
    2	325.4 on Ele 109958	278.7 on Ele 107683	264.2 on Ele 105331	0.00138 on Ele 104299	0.00125 on Ele 107630	0.00119 on Ele 105331

CONCLUSION: 

1. Spot welds were modeled using both 1d beam elements as well as 3d Hexa elements. The spot welds modeled using the Hexa elements transferred more forces across the joining parts as a result of its higher stiffness.
2. The solver deck was set-up for the crash simulation and the required results were requested using the appropriate *DATABASE keyword cards.
3. The analysis ran successfully. Post-processing of the results was done using the D3plots and the other output ASCII result files, to produce the deliverables.

Click here to view the completed files.