Modelling Spotwelds using LS-DYNA

Aim:

To model the spot-weld for the given assembly parts using beam and solid elements separately.

2) To perform the crash analysis for the same and compare the output results of the beam and solid spot-welds.

Procedure:

Importing the Model:

1) We first open the LS Prepost software and import the keyword file (.k file).

2) The keyword file consists of sheet metal plates that have to be joined using spot welds as shown in the image given below.

+

Assigning Section:

3) Since the Sheet Metals are meshed using 2d elements we will define them with the SECTION_SHELL card. We also parallelly assign section properties i.e. 1.5 mm thickness to the sheet metal plates as well.

Here,

1. SECID: Section ID. SECID is referenced on the *PART card. A unique Number or label must be specified.
2. ELFORM: Element formulation options.=16 Fully integrated shell element (very fast)
3. SHRF: Shear correction factor which scales the transverse shear stress.= 1
4. NIP: Number of through-thickness integration points = 2
5. T1: Shell thickness =1.5 mm

Assigning Material:

4) We are supposed to Create Two material cards one for the sheet metal and the other for spot weld. We are using MAT_ELASTIC card for Sheet metal using Steel Properties and the unit system followed for the unit consistency is gm-mm-ms.

Here,

1. MID: Material identification. A unique number or label not exceeding 8 Characters must be specified.
2. RO: Mass density = 0.00785`(gm)/(mm^3)`
3. E: Young’s modulus = 2.10 e+05 `(gm)/(mm* ms^2)`
4. PR: Poisson’s ratio=0.3

Assigning Materials and Sections to Parts:

5) We specify the respective Material and Section ID to the bottom and top sheet metal part IDs.

Rigid Wall Creation:

6) Next step is to create a Rigid wall in front of the top sheet metal part 15 mm away by using the *RIGIDWALL_PLANAR card. This is done by selecting Entity Creation > RigidWall > Create. The rigid wall type is selected as a Planar and defined vector with one point and a normal ie, 1n+NL here selected the one node, and the normal is created as a rigid wall. This rigid wall is translated/offset by 15mm from the crash box component.

Initial Velocity:

7) Next step is to define a velocity of 50kmph (13.8889 mm/ms) and assigned it to each node of the selected bottom and top sheet metals, under Entity Creation >Initial>Velocity>Insert the value. The bottom and top sheet metals are selected by pick option concerning part as shown below.

Here,

1. NSID: Node Set ID, we already created the node-set for the floor.
2. VX: Velocity along Translational X-axis.
3. VY: Velocity along Translational Y-axis.
4. VZ: Velocity along Translational Z-axis.
5. VXR: Velocity along Rotational X-axis.
6. VYR: Velocity along Rotational Y-axis.
7. VZR: Velocity along Rotational Z-axis.

Control Cards:

8) The spot-weld can be modeled as beam and solid elements by using the following techniques,

• To represent as a beam element, we use *CONTROL_TIED_SHELL_EDGE_TO_SURFACE card
• To represent as a solid element, we use *CONTROL_SPOTWELD card

Spot-weld modeled using Beam element:

9) The spot weld modeled using beam element is created by selecting the Mesh > Element Generation > Beam > Give Part ID > Select Beam by Two_Node_Sets > Pick Node set 1 & 2 (pick the desired nodes from the bottom and top sheet metal) > Create > Accept > Done. Now this beam element acts as a spot weld.

10) Here the fact is that automatically a Section card (*SECTION_BEAM) and the Material card (*MAT_CABLE_DISCRETE_BEAM) are created and we need to delete these cards and assign our required material and section cards.

Defining the Material card for Beam Element:

11) For the beam element, the material card is assigned as the *MAT_100 that is especially for the spot weld material. The values are assigned and here we are taking a time-dependent failure concept rather than the force-dependent failure concepts like Effective plastic strain, maximum axial stress, maximum shear stress, Force resultant, Torsional moment resultant, Moment resultant. So to keep this problem as a Time-dependent failure we given other failure terms as a higher value.

Here,

1. MID: Material identification. A unique number or label not exceeding 8 characters must be specified.
2. RO: Mass density
3. E: Young’s modulus.
4. .PR: Poisson’s ratio
5. SIGY: Initial yield stress
6. TFAIL: Failure time if nonzero. If zero this option is ignored.
7. EFAIL: Effective plastic strain in weld material at failure
8. NRR: Axial force resultant 𝑁𝑟𝑟 at failure.
9. NRS: Shear Force resultant 𝑁𝑟𝑠𝐹 at failure
10. NRT: Force resultant 𝑁𝑟𝑡𝐹 at failure
11. MRR: Torsional moment resultant 𝑀𝑟𝑟𝐹 at failure.
12. MSS: Moment resultant 𝑀𝑠𝑠𝐹 at failure
13. MTT: Moment resultant 𝑀𝑡𝑡𝐹 at failure.

Defining the Section card for Beam Element:

12) For the beam element, the section property is assigned by using the *SECTION_BEAM card. It is important to assign element formulation (ELFORM) as 9 because the *MAT_100 spot weld material model only applies for ELFORM 9 formulation in the case of the beam element. The cross-section type is selected as tubular since the default cross-section(rectangular) gives zero cross-section area during the simulation and the beam thickness at both ends is given as 3mm.

Here,

1. SECID: Section ID. SECID is referenced on the *PART card. A unique Number or label must be specified.
2. ELFORM: Element formulation options.= 9 spotweld beam
3. SHRF: Shear correction factor which scales the transverse shear stress.= 1
4. QR/IRID: Quadrature rule or rule number for the user-defined rule for integrated beams.
5. CST Cross section type = 1 Tubular
6. TSI Beam Thickness = 3.0mm

Assigning Materials and Sections to Parts:

13) We specify the respective Material and Section ID to the spotweld IDs.

Defining the Contact card for Beam Element:

14) Here for the beam element, the contact type to be used is *CONTACT_TIED_SHELL_EDGE_TO_SURFACE card and the master set id will be Part id and the Slave set id will be nodes of beam weld element. For defining the Slave set select beam nodes to create the set and the steps are mentioned below,

Entity Create > SetData > *SET_NODE > Pick the nodes > Apply.

For defining the Master set select both the metal sheet parts and the steps is mentioned below,

Entity Create > SetData > *SET_PART > Pick the part > Apply.

So assign both the slave-set and the master-set as created by the above technique to the contact card. *CONTACT_TIED_SHELL_EDGE_TO_SURFACE card.

Slave-type - Node set ID

Master-type - Part set ID

15) Also we need to create an Automatic_single_surface contact card for the parts to ensure that after the spot weld breaks the parts come to each other they shouldn't penetrate. Here the parts-sets are the slaves.

Spot-weld modeled using Solid element:

16) The spot weld modeled using solid element is created by selecting the Element Tools > Element Editing > Create > Type - Hexa > Pick four desired nodes from the bottom and top sheet metal > Accept > Done. Now this solid element act as a spot weld.

Defining the Material card for Beam Element:

17) For the beam element, the material card is assigned as the *MAT_100 that is especially for the spot weld material. The values are assigned and here we are taking a time-dependent failure concept rather than the force-dependent failure concepts like Effective plastic strain, maximum axial stress, maximum shear stress, Force resultant, Torsional moment resultant, Moment resultant. So to keep this problem as a Time-dependent failure we given other failure terms as a higher value.

Here,

1. MID: Material identification. A unique number or label not exceeding 8 characters must be specified.
2. RO: Mass density
3. E: Young’s modulus.
4. .PR: Poisson’s ratio
5. SIGY: Initial yield stress
6. TFAIL: Failure time if nonzero. If zero this option is ignored.
7. EFAIL: Effective plastic strain in weld material at failure
8. NRR: Axial force resultant 𝑁𝑟𝑟 at failure.
9. NRS: Shear Force resultant 𝑁𝑟𝑠𝐹 at failure
10. NRT: Force resultant 𝑁𝑟𝑡𝐹 at failure
11. MRR: Torsional moment resultant 𝑀𝑟𝑟𝐹 at failure.
12. MSS: Moment resultant 𝑀𝑠𝑠𝐹 at failure
13. MTT: Moment resultant 𝑀𝑡𝑡𝐹 at failure.

Defining the Section card for Solid Element:

18) For the solid element, the section property is assigned by using the *SECTION_SOLID card. It is important to assign element formulation (ELFORM) as 1 because the *MAT_100 spot weld material model only applies for ELFORM 1 formulation in the case of the solid element.

Here,

1. SECID: Section ID. SECID is referenced on the *PART card. A unique Number or label must be specified.
2. ELFORM: Element formulation options.= 1 solid element.

Assigning Materials and Sections to Parts:

19) We specify the respective Material and Section ID to the spotweld Hexa element IDs.

Defining the Contact card for Solid Element:

20) Here for the solid element, the contact type to be used is the *CONTACT_SPOTWELD card and the master set id will be Part id, and the Slave set id will be nodes of solid weld element.

For defining the Slave set select solid nodes to create the set and the steps are mentioned below,

Entity Create > SetData > *SET_NODE > Pick the nodes > Apply.

For defining the Master set select both the metal sheet parts and the steps is mentioned below,

Entity Create > SetData > *SET_PART > Pick the part > Apply.

So assign both the slave-set and the master-set as created by the above technique to the contact card. *CONTACT_SPOTWELD card.

Slave-type - Node set ID

Master-type - Part set ID

21) Also we need to create an Automatic_single_surface contact card for the parts to ensure that after the spot weld breaks the parts come to each other they shouldn't penetrate. Here the parts-sets are the slaves.

Control Cards:

22) Control­_Termination is defined at what time the simulation ends or the end time of the simulation and it is set to 5 ms.

Here,

ENDTIM: It is the time at which the simulation ends.

23) Control_Energy provides controls for energy dissipation options.

Here,

1. HGEN: Hourglass energy calculation option. Is set to 2 In Which hourglass energy is computed and included in the energy balance.
2. RWEN: Rigid wall energy dissipation option: Is set to 2 in Which energy dissipation is computed and included in the energy balance.
3. SLNTEN: Sliding interface energy dissipation option Since the Contact is Defined it is set to 2 so that energy dissipation is computed and included in the energy balance.

Database Creation:

24) BINARY_D3PLOT is defined as the frequency at which the animation file is to be created and is set to 0.5 ms.

Here,

DT: Time-frequency at which the animation files should be printed.

25) For generating section forces creating a specific node and element/shell list which defines the desired section of component is necessary. The selection of nodes and elements/shell lists is done by picking each node and element through Creating Entity>Set Data>*SET_NODE for node-set and Creating Entity>Set Data>*SET_SHELL for element/shell-set.

Here,

1. NSID: Node Set ID.
2. SSID: Shell Set ID.

26) We take history for beam and solid elements for measuring axial and shear forces on the beam and solid elements

27) The nodes along the beam and solid elements were defined to measure the acceleration using the DATABASE_HISTORY_NODE.

28) ASCII_option keyword is the output request in ASCII format, The following keywords are Activated.

1. ELOUT: Element Data
2. GLSTAT: Global Data
3. MATSUM: Material Energies
4. SWFORC: Spotweld Nodal Constraint Reaction Forces
5. NODOUT: Nodal point data
6. SECFORC: Cross-section forces

Keywords:

29) Finally, we have set up the simulation model for both cases and have a final look at our keyword manager which contains all the necessary parameters for running the simulation.

Model Check:

30) We perform model checking to find any errors or warnings present simulation model.

Results and Discussion:

1) We save the LS Dyna keyword file in a different folder and we go to the LS-Run Manager and run the simulation by importing the LS Dyna keyword file. The simulation finishes successfully with a normal termination. We then go to lsrun.out file and open it with a text editor to see the time taken for both beam and solid spotweld models to complete the simulation.

Contour Animation:

2) The von Mises yield criterion states that if the von Mises stress of a material under load is equal or greater than the yield limit of the same material under simple tension then the material will yield. In both the simulation the component hits the rigid wall at 1.0799ms of the simulation, the spotweld fails, exactly half the termination time ie, 2.5ms. There is no abnormal behavior of elements during the simulation since the element's materials are defined using the elastic property. After the spot weld fails we can see that the top and bottom parts come into contact and causing the stress at the contact area and which is shown in the below contour as a red-colored region.

Output Results:

GLSTAT - Global Energies plot

3) From the plots above ie, the study of the beam and solid weld, here initially the sheet metal parts had a velocity of 13.8889mm/ms and as they impacted the rigid wall we can able to see that the Kinetic Energy of the component is been decreased and between in terms internal energy of the component is been increased higher and the hourglass energy is fall to zero as we controlled it in both the case study. The total energy of the system remains constant.

NODOUT - To find the Nodal motions

Here the nodes are selected from the top and the bottom part of the sheet metal A-node represents the top part node and B-node represents the bottom part node. It can be seen that after the impact the acceleration is not constant, at first the acceleration values decreases due to a drop in velocity of the component ie, acceleration (-ve velocity), and then goes up and down as shown in the figure above. The top metal sheet bounces back due to the impact whereas the lower metal sheet part connected with the spot weld continues to travel in the same direction due to momentum from the top part.

SWFORC - To find Spotweld Beam & Solid Axial and Normal Forces

Here the study was carried out by modeling the spot weld at the 7 locations ie, 2 numbers each at the left and right sides as shown in the above figures and 3 numbers at the top side so that the top and bottom metal sheet parts are held together. The problem with the beam element is that it takes load only in one direction as focussed and shear load is not easily understandable from the results. So in the above figure too, we can see that the higher axial forces can be seen compared to shear forces for spot welds modeled by the 1D beam element. The force values drop to zero after the spot weld fails (ie, after 2.5ms). Whereas, higher shear forces are notices comparatively to axial forces for spot welds modeled by solid element. The force acting on the spot weld is in the transverse direction (perpendicular to the axis) since the solid element gives the force-resisting ability in the transverse direction, higher shear force values are notices for a solid element than a beam element.

Conclusion:

1) The spot welds are modeled using Beam and Solid elements for the same component.

2) The material card and all other keywords are properly defined for the simulation.

3) The simulation carried out with time-dependent failure and the spot weld is failed at half of the termination time.

4) The component bounces back after impacting on the rigid wall.

5) The plot results and contour diagrams are compared.