Eliminating Contact Force Interference in Spotweld Forces Using SPOTTHIN in *CONTROL_CONTACT

In mesh independent deformable spotwelds (see here ), the actual spotwelds are represented using either beams or solids (single or cluster). The nodes of the beam or solid element representing the spotweld are then tied to the sheet metal using a tied interface (TIED_SHELL_EDGE_TO_SURFACE or TIED_NODES_TO_SURFACE). The forces experienced by the beam are the result of this tied interface and then the stiffness of the beam element. A simple spotweld modeling using beam element is shown below.

(Click to Enlarge)

In certain situations due to large deformations, the segments on sheet metal already used in the tied interface could interact with regular contact-impact treatment for example when using a global AUTOMATIC_SINGLE_SURFACE contact definitions in which the thickness offsets are always considered. The interference of the contact forces due to the offset with the beam forces could prematurely cause the beam or the solid element to fail or lead to incorrect forces in the weld element as shown below.

(Click to Enlarge)

To overcome the influence of contact-impact forces with the actual tied interface, one can use SPOTTHIN parameter using *CONTROL_CONTACT which allows the user to scale ALL the segments already used in the tied interface by a factor of SPOTTHIN of the original segment thickness. This basically has the effect of simply not allowing the segments to interact due to small thickness. Since SPOTTHIN is a scale factor, it can carry a value of 0 (no scaling) to 1.0 (100% scaling) down of the original thickness. This is shown below.

(Click to Enlarge).

Optionally, one can increase the area of the segment search that is to be “thinned” by increasing the radius of the beam or the solid using the parameter SWRADF. When SPOTTHIN is greater than zero and SWRADF is greater than zero, LS-DYNA loops through all the segments that are attached to the segment used to tie the beam to and scales those segments thickness as well. This is shown below.

(Click to Enlarge)

Deformable Spotwelds in LS-DYNA

Over the years, spotweld representation for crash and NVH applications have evolved from a crude to a detailed modeling resulting in reduced pre-processing effort while greatly enhancing the accuracy of numerical models. Here is link that gives a brief overview of spotwelding process in LS-DYNA. Please note that the document is over 2 years old and has not been updated since. Please refer to the latest LS-DYNA keyword and theory manual for more information.

Deformable_Spotwelds_in_LS-DYNA_for_Impact.pdf

Additional information compiled by Mr. Jim Day: Spotwelds

Limitations of Penalty Joint Treatment in LS-DYNA

LS-DYNA supports various joint definition types such as spherical, cylindrical, etc (please refer to the LS-DYNA User’s manual for a complete list). Irrespective of the joint definition type and the elements associated, translational constraints are applied to the joint nodes to model appropriate behavior. The constraints are applied using the default penalty formulation whose stiffness depends on the maximum frequency of all joints in the model, timestep and the timestep-scale-factor (TSSFAC). The default penalty formulation computes the necessary forces in an attempt to model the joint behavior based on the joint type but in some instances the forces generated by the penalty treatment may be insufficient to maintain the constraint. As a good practice, it is always recommended to monitor the relative displacements between the joint nodes to see if there is any separation which would indicate a insufficient forces being generated by the penalty treatment. There are two ways to fix if there is some relative displacement between the nodes. The first approach would be to increase the penalty scalefactor RPS in *CONTRAINED_JOINT keyword whose value is based on trial-and-error appraoch. The second approach is to switch the penalty formulation to an implicit Lagrange-Multiplier formulation which computes the exact force to enforce the joint constraint. Beginning 971 and onwards, this option is now available for both SMP and MPP versions of LS-DYNA and can be invoked using the *CONTROL_RIGID keyword using the parameter LMF.