Modelling and Analysis of Beam and Solid Spotwelds on Crashbox

Objectives:

• To model the spotwelds and simulate a crash test for which the meshed file has already been given.
• Two types of spotwelds have to be modeled viz. using beam elements and using solid/hexa elements on the crashbox at the region specified in the challenge, in a symmetric manner. The number of spotwelds should be kept between 3-7.
• The failure time for the spotweld has to be defined as half of the time of the actual simulation. The material for both the spotwelds has to be assigned using the material card *MAT_SPOTWELD.
• To compare the axial and shear force in the spotwelds for both the beam and solid elements. The solid spotweld should be created using only one hexa element.
• A rigid wall has to be created in front of the crashbox and the crashbox has to be impacted on the rigid wall with a velocity of 50kmph, and the spot welds have to be analyzed for their failure.
• Show plots of energy, section force at the spotweld region, effective stress, effective plastic strain, acceleration of the middle node of the beam, axial and shear forces in the spotweld. This is applicable for both the spotwelds.

Introduction:

• Spotweld is a common welding method used to join two or more metal components at a particular spot, unlike other welding methods where the weld is created along a line. 
• In FEA, spotweld is used as a connection to connect multiple parts. It is modeled as either a 1D joint or a 3D (hexa) joint. Modeling a spotweld as a 1D element, reduces the computational time and cost, while the 3D joint gives more freedom in the actual representation of the weld, but at the expense of time and cost.
• There are a number of spotwelds in a vehicle assembly for eg, and in such cases, the type of the spotweld plays an important role. Therefore, in the regions where the behavior of the spotwelds is not crucial, the 1D type is preferred. While in the areas where a spotweld may determine the failure of a certain component, a solid spotweld is used.
• There are 4 methods to model any spotweld in "LS-DYNA":
  • Beam element using the *CONTACT_TIED_SHELL_EDGE_TO_SURFACE
  • Using the *CONSTRAINED_SPOTWELD keyword
  • Using the *CONSTRAINED_GENERALIZED_WELD_SPOT
  • Using solid elements and *CONSTRAINED_SPOTWELD keyword
• In this challenge, the 1st and the last method has been used to model the spotwelds. Altogether, 5 spotwelds have been applied on the beam, 2 at both the sides and 3 along the width of the beam. 
• There are 3 MAT100 spotweld material keywords for modeling a spotweld. But here the *MAT_SPOTWELD has been employed. This material model has been specified according to the properties of steel.
• Apart from this, all the deliverables are similar to the week 4 challenge of the crashbox. 

Procedure:

• The model was provided in the .k format which was opened in the "LSPP" and the image below shows the meshed model as provided in the challenge.
  
  
  
  
• The unit system that had to be followed throughout the analysis was 'gm mm ms', and the material for the spotwelds and the part was specified as steel.
• Initially, the spotwelds were created using the beam elements. 5 beams were created over the crashbox using the 'mesh>ele edit>create>'. Here the element type was selected as 'beam'. Two nodes were selected to specify the beam, one on the top part and the other on the bottom part. A separate PID was created for the beam automatically.
• Following the same line of the elements and the symmetry, 5 such beams were created, 2 on both left and right side of the crashbox and 3 on the top of the crashbox.
  
  
• After creating the 5 beams, a material was assigned to them. This was done by creating a MAT100 *MAT_SPOTWELD keyword from the 'keyword manager'. The *MAT_SPOTWELD keyword was modeled based on the properties of steel. The values of density (RO), Young's Modulus (E), Poisson's ratio (PR), and yield strength (SIGY) were set according to the steel material card in the unit system of gm mm ms. 
• As mentioned in the deliverables, the beam was supposed to fail exactly at half of the termination time. Since the termination time, in this case, was decided as 10ms, the TFAIL value was set as 5ms. The EFAIL that is the effective plastic strain rate at failure was set as a high random value of 10 since the failure criteria had to be time-based. Similarly, the NRR, NRS, NRT, MRR, MRS, MRT, were specified with high magnitude.
• A trial simulation was performed on the crashbox without the TFAIL criterion, and a random high value of forces, to get an idea as to how much force magnitude was required for the beam spotwelds to fail for the same velocity of impact. Based upon this trial simulation, the values of NRR, NRS, NRT, MRR, MRS, MRT, were decided. They were kept higher than the force values at which the beams were failing during the trial, in order to induce a time-based failure. The image below shows the material keyword for the actual simulation. 
  
  
  
  
• After the creation of the material for the beam, the material keyword for the shell elements of the top and the bottom part was created. The material properties for this keyword too, was set as Steel.
  
  
  
  
• Later, section for the beam had to be defined. For this purpose, the *SECTION_BEAM keyword was used. The MAT100 which was defined for the beam is only applicable for the beam section with element formulation type 9. Hence the ELFORM value was set as 9, while the CST (cross section type) was set as 1 (Tubular). The TS1 and TS2 (outer dia at node 1 and 2) was set as 2.0mm. The image below shows the section card.
  
  
  
  
• Similarly, a section keyword *SECTION_SHELL was created for the crashbox shell elements, with ELFORM 2, and thickness 1.5, as seen in the image below. 
  
  
  
  
• After creating the material and section for both the beam and the crashbox, they were specified in the *PART keyword for the respective parts.
  
  
  
  
• A contact had to be defined between the beams and the shell elements. But for that, a set of nodes for the beams had to be created. A separate *SET_NODE was created from the 'create entity' option, in which all the nodes of the beams were defined.
  
  
  
  
• Similarly, a *SET_PART was created for both the top and bottom pat of the crashbox.
  
  
  
  
• Since the spotwelds were being created using the beam elements, it was necessary to create a contact keyword to define the contact between the beam and the shell elements. *CONTACT_TIED_SHELL_EDGE_TO_SURFACE was created from the 'keyword entity' option. In this contact keyword, a SSID (slave set ID) and MSID (master set ID) had to be defined. The slave elements were the beams since they are the connecting elements between the two parts and are more deformable than the crashbox, while the master set was the crashbox. Sinc the node set for the beams had already been created, the SSTYP was changed to 4 (node set ID) and the node set was selected in the SSID. For the MSID, the part set was created. Hence, the MSTYP was changed to 2 (part set ID) and the part set was selected in the MSID.
  
  
  
  
• In the material keyword MAT100, the TFAIL time was defined as 5ms. Hence, the beam spotweld was set to break at the 5th ms. Because of this, there was a possibility that the top and the bottom part may come in contact with each other. Therefore to avoid the errors and numerical instability in the analysis, a self contact had to created between the two parts of the crashbox. This was done by creating a *CONTACT_AUTOMATIC_SINGLE_SURFACE was created and the part was defined in the SSID (there was no need to define the MSID as it was a self contact). 
  
  
  
  
• Later, a rigid wall had to be created in front of the crash box onto which the crashbox would hit. This was done by creating a planar rigid wall in front of the top part of the crashbox. From the 'create entity' option, the 'rigid wall' was selected and the middle node of the face of the top part selected. A gap of 10mm was set to visualize the impact of the crashbox in the X-direction.
  
  
  
  
  
  
• The crashbox had to be impacted on the rigid wall at a velocity of 50kmph. But since the unit system that was followed throughout the simulation was gm mm ms, the magnitude of the velocity was changed to 13.88mm/ms. The initial velocity was applied from the 'create entity>initial>velocity>cre'. In the X-direction, a magnitude of -13.88 (towards the centre) was defined and the initial velocity was applied.
  
  
  
  
• In the output requests, the cross-sectional force of the middle section of the crash box containing the beams had to be plotted, a node-set containing the middle nodes (along with the beams) was created from 'create entity>set data>*SET_NODE>cre'. Similarly, a *SET_SHELL was also created containing the elements in the same region.
  
  

Output Requests: 

• *CONTROL_TERMINATION: a control termination keyword was created with a termination time of 10ms for the simulation.
  
  
  
  
• *DATABASE_CROSS_SECTION_SET: was created from the 'keyword manager' for the cross-sectional force. The NSET created at the middle region was defined in this keyword.
  
  
  
  
• *DATABASE_BINARY_D3PLOT: for the database of the model was created with a DT of 0.5ms, which meant that the database files would be created at every 0.5ms interval.
  
  
  
  
• *DATABASE_ASCIIOPTION: was created for the ascii files of glstat, matsum, rcforc, rwforc, secforc, sleout, and swforc, each with a DT of 0.1. The swforc was created in order to get the spotweld forces.
  
  
  
  
• After the case setup and output request setup, the keywords in the model were checked for any errors present in it. This was done using the 'model check' option present in the 'keyword manager'.
  
  
  
  
• After confirming that the model was free of any errors, the simulation was run by importing the .k file in the "LSRUN", and then it was evident from the simulation that the beam spotwelds failed exactly at 5th ms.
  
   
  
  
• The d3plot was opened in LSPP and the animation of the simulation was observed. The beam spotwelds were deleted from the model in the middle of the simulation. The Von-Misses stress contour was plotted, and the maximum amount of the Von-Misses stress induced in the crashbox was 481.3MPa.
  
  
  
  

Solid Spotweld (Hexa):

• The beam spotwelds were replaced with the solid spotwelds after the analysis of the beam elements. The solid/hexa elements were created by using the same option for the beam elements except the 'beam' option was replaced with the 'hexa' option from the 'mesh>ele edit>cre>hexa' by selecting 4 nodes on each part.
  
  
  
  
• The hexa elements created for the spotweld were defined in a separate node-set from the 'create entity' option, in order to specify them in the contact keyword. The material for the spotweld was kept constant, and only the section of the spotweld was changed to *CONTACT_SPOTWELD. 
  
  
  
  
• Along with this, the section of the spotweld was also changed from *SECTION_BEAM to *SECTION_SOLID since the spotweld was created as hexa elements. The ELFORM was set as 1- constant stress solid element.
  
  
  
  
• Keeping all the other keywords and entities constant, the .k file was simulated in the LSRUN, and similarly to the previous simulation, the solid spotwelds failed exactly at the 5th ms.
  
  
  
  
• The d3plot was opened in the LSPP and the Von-Misses stress contour was plotted, and the maximum value of the Von-Misses stress value induced in the model was 573.1MPa.
  
  
  
  
• The axial forces induced in the spotwelds for both the beams and the solid were plotted from the 'ascii option' from the 'post' tab and the maximum amount of axial force generated in the beam spotwelds was around 875N, and the same in the solid spotwelds spiked at 900N. But the overall/average axial force was higher in the beam spotweld, since the beam has higher tensile strength and thus takes higher tensile loads.
  
   
  
  
• Similarly, the shear forces were also plotted for the beam and the solid spotweld. The maximum value of the shear force in the beam spotwelds was around 475N while that in the solid spotweld was around 1900N. This was because of the solid element used in the spotweld.
  
   
• Sectional forces in the beam and the hexa spotweld are plotted below. There was a slight difference between the maximum values of the sectional forces for both the crashboxes. The highest value of sectional force for the beam spotweld was 50000N and for the solid spotweld, it was around 55000N.
  
   
  
  
• Effective Plastic Strain was calculated at the same element for both the spotwelds i.e. 102632. This was done from the 'history' tab, and selecting the element number. Both the plots are exactly the same.
  
   
  
  
• Similarly, the effective stress (von-misses) was calculated for the same node no. 102632. The maximum effective stress was also the same in both the spotwelds, but the overall average value of the stress increased in the solid spotweld as the simulation progressed compared to the beam spotweld.
  
   
  
  
• The plot for the acceleration of the middle node was plotted. The number of the node was 502711. The maximum acceleration was seen in the solid spotweld which was around 47.5mm/ms^2 at the 6th ms. While the beam spotweld had the maximum acceleration of around 36mm/ms^2 at the 1st ms.
  
   
  
  
• Later, the 'glstat' file was loaded in the 'ASCII' option for both the spotwelds. The plot for the kinetic energy, internal energy, total energy, hourglass energy, and sliding energy was drawn. It was observed that the internal energy for the solid spotweld was higher as compared to the beam spotweld, and peaked at a value of around 1.12E^6 Nmm, though the total energy remained constant at 1.4E^6 Nmm. On the other hand, the kinetic energy was higher at the end of the simulation in the beam spotweld with a value of around 0.48E^6 Nmm, while the internal energy in the solid spotweld dropped to a low value of 0.25E^6 Nmm. As compared to these energy values, the hourglass energy in both the spotwelds was negligible, and the sliding energy was 0 throughout the simulation.
  
   
  
  

Conclusion:

• In this challenge, the crashbox connected using the two types of spotwelds were analyzed successfully and the results were plotted. The types of spotwelds used for structural analysis are of 2 types viz. 1D spotweld and 3D spotweld. 1D spotwelds are generally modeled using the beam elements while the solid spotwelds are modeled using the hexahedral elements. 
• There are 4 methods that are used to model a spotweld in "LS-DYNA":
  
  • Beam element using the *CONTACT_TIED_SHELL_EDGE_TO_SURFACE
  • Using the *CONSTRAINED_SPOTWELD keyword
  • Using the *CONSTRAINED_GENERALIZED_WELD_SPOT
  • Using solid elements and *CONSTRAINED_SPOTWELD keyword
• In this challenge, the 1st and the last method were used along with the respective types of contacts. Both the spotwelds were modeled as steel using the material keyword MAT100 i.e. *MAT_SPOTWELD. The unit system which was followed throughout the challenge was gm mm ms. The crashbox had to be impacted on a rigid wall, at a velocity of 50kmph or 13.88mm/ms. After creating the spotwelds and the relevant keywords, the model was simulated in "LSRUN".
• After the simulation, it was observed that the stress generated in the solid spot-welded crashbox was higher than the beam spot-welded crashbox. 
• The shear forces in the spotweld were higher in the case of solid spotweld, while the axial forces were almost the same. But the beam spotweld had a higher overall axial force. The reason behind this was the beam has higher tensile resistance and can take higher axial forces. Along with this though the total energy was the same in both the models, the internal energy was higher in the solid spotweld. 
• The failure of both the spotwelds was scheduled at half of the termination time (5ms) and behaved as desired.

GDrive Link for the models and files: BEAM AND SOLID SW