The general procedure for defining a spot weld set consists of the following steps:
In addition, the SWLIST and SWDEL commands are available for listing and deleting spot weld sets.
Use the SWGEN command to define a basic spot weld set (in the GUI, pick ). The required arguments are:
Name of the spot weld set
Spot weld radius
Spot weld surfaces
First spot weld node
You can optionally specify the following:
Second spot weld node
Spot weld projection direction
Search radius
Contact and target element types
All of these inputs are discussed in detail below.
Ecomp):Use the Ecomp argument to assign a name to
a new basic spot weld set. The spot weld set is a component composed of
new beam, target, and contact elements. The name entered for
the Ecomp argument will be used to list,
delete, output, or add new surfaces to the spot weld set.
NCM1,
NCM2):Each basic spot weld set contains two surfaces, surface 1 and surface
2, to be connected together. Use arguments
NCM1 and NCM2
to specify these surfaces. You can input the name of a predefined node
component or a meshed area number. If no nodal component names matching
NCM1 and NCM2
are found, they are assumed to be meshed area numbers.
SND1,
SND2):You must specify the first spot weld node,
SND1. The location of each spot weld depends on
SND1. If you specify the second spot weld
node (SND2), it is used to determine the spot
weld projection direction. The second node will be generated
automatically if it is not specified. You should locate
SND1 and SND2
(referred to as node 1 and node 2 in figures that follow) as close to
the corresponding surfaces as possible. They can be nodes on the
corresponding surfaces or independent nodes in space. If they are not on
the corresponding surfaces, node 1 will be moved to surface 1 and node 2
will be moved to surface 2.
The program determines the actual location for the spot weld nodes by first projecting node 1 onto surface 1 along the spot weld projection direction. Next, the program projects node 2 to surface 2 along the spot weld projection direction. The spot weld nodes are moved to the surfaces in the beginning of the analysis.
By default, the projection direction is a surface normal vector from
node 1 to surface 1 (see figure below). If you specify node 2
(SND2), the projection direction is in
line with the two spot weld nodes. If node 2 is not specified, you can
still explicitly define the projection direction with the
DIRX, DIRY,
and DIRZ arguments.
Once the actual location of node 1 has been determined, the program projects node 2 to surface 2 along the spot weld projection direction that was used for node 1. The figure below shows the projection locations of nodes 1 and 2 given a default projection normal to surface 1.
The figure below shows spot weld node 1 projected as specified by the
user (either through the input of DIRX,
DIRY, and
DIRZ, or by the specification of a second
spot weld node).
The figure below is another example showing the projection location of spot weld nodes 1 and 2 given a user-specified projection direction.
SWRD):Each spot weld is assumed to have a circular projection onto the spot
weld surfaces. The projection is defined by the required spot weld
radius argument SWRD. For each spot weld
surface, the program builds six force-distributed constraint equations
through a contact pair. The spot weld radius determines the influence
range of the constraint equations. Each spot weld node couples with a
group of nodes on the corresponding surface within the radius. (See
Figure 12.7: Nodes Included in Constraint Equations later in this section.)
SHRD):The program creates a contact pair for each spot weld surface. The
contact pair contains one contact element defined by the spot weld node,
and target elements overlaid fully or partially on the corresponding
spot weld surface. Only the surface nodes that fall within a sphere of
radius, called the search radius, with its center at the original
position of the corresponding spot weld node are used to form target
elements (see figure below). The search radius must be larger than the
spot weld radius. If the search radius argument
(SHRD) is not defined, the program uses a
default search radius that is four times the spot weld radius.
ITTY,
ICTY):By default, the program automatically creates the target and contact
element types required for the spot weld. However, you may use the
ITTY and ICTY
arguments to specify the target and contact element types, respectively.
You must also set certain key options if you specify the element types
to be used. See The Components of a Spot Weld for more
information.
Each new spot weld set created by the SWGEN command consists of a beam element and two node-to-surface MPC contact pairs (see Modeling a Shell-Solid Assembly for more information). Each node-to-surface pair will generate 6 constraint equations. You can choose either a rigid MPC184 element (the default) or a deformable BEAM188 element to link the spot weld surfaces. Below are detailed explanations of how these items are generated:
Contact Pairs: Two node-to-surface contact pairs are created for each new spot weld set. One pair is for spot weld surface 1 and the other is for surface 2. Each contact pair has only one contact element, CONTA175, which is defined by the associated spot weld node. The target elements (TARGE170) are formed by a group of surface nodes lying within the region of the search radius. The program creates an independent real constant ID for each contact pair, and proper contact and target element type IDs.
If you prefer, you can specify the contact or target element type IDs to
be used. To specify a contact element type, use the
ICTY argument on SWGEN and set the
following contact element options for that element type: KEYOPT(2) = 2 (MPC
approach), KEYOPT(12) = 5 (bonded always). To specify a target element type,
use the ITTY argument on SWGEN
and set the target element option KEYOPT(5) = 4 (force-distributed
constraint, all directions) for that element type.
Force-distributed constraint equations: For each contact pair, the program internally forms force-distributed constraint equations that distribute the internal forces of the spot weld node (that is, the contact node) to the surface nodes (that is, the target nodes) lying within the region of the spot weld radius. This includes all elements that fall entirely or partially within the radius (see the figure below). In other words, it couples the motion of certain surface nodes to the motion of the spot weld node (in an average sense). There are six constraint equations generated for each spot weld surface (that is, each contact pair).
Beam element: A beam element is created to connect spot weld surface 1 and surface 2. The two beam end-nodes are the spot weld nodes, node 1 and node 2 (see Figure below). The spot weld set can be rigid or deformable. By default, the program creates a rigid beam element (MPC184 with KEYOPT(1)=1) to represent a rigid spot weld. However, if the currently defined element type is BEAM188 with a solid circular cross-section, the program assumes the spot weld set is deformable and a BEAM188 element is created. In this case, you must input the material properties with the MP command and define the geometry of the beam section using the SECTYPE and SECDATA commands (see the example listing below). Generally, BEAM188 is capable of handling a short beam situation.
The following example input shows typical commands used to define a spot weld with a deformable BEAM188 element having a circular cross section.
MP,EX,3,200000000000. ! spot weld material properties
MP,NUXY,3,0.3
SECTYPE,3,beam,csolid ! define a circular solid beam section
SECDATA,2.75e-002 ! beam circular radius
ET,3,188 ! element type for a deformable spot weld
TYPE,3
MAT,3
SECNUM,3
*SET,NODE1,9000 ! define parameter for node number
N,NODE1,0.1,0.5,10.2 ! define spot weld node
SWGEN,SWELD1,2.75e-2,2,3,NODE1 ! Spot weld name = SWELD1
! Radius = 2.75e-2
! Spot weld surfaces = areas 2 and 3
Note: All limitations that are documented for the MPC184 link/beam element in the Element Reference also apply when the element is used in a rigid spot weld definition. Please read the MPC184-Link/Beam description carefully, especially the assumptions and restrictions.
Once a basic spot weld set has been created, additional surfaces can be added to
the existing spot weld set. Use the SWADD command to define the
additional surfaces (in the GUI, pick ).
Each added surface (input as NCM1 through
NCM9) can be specified by an existing nodal component
name or by a meshed area number.
In the example command below, four surfaces are added to an existing spot weld set named SWELD1. The four surfaces include area number 3, area number 4, nodal component FAC5, and nodal component FAC6. The search radius is 0.8.
SWADD,SWELD1,0.8,3,4,FAC5,FAC6 ! Adds 4 surfaces to spot weld SWELD1.
For each new surface, the program creates a new spot weld node, a new contact
pair, and a new beam element (see figure below). The location of the new node is
determined by projection of one of the closest existing spot weld nodes onto the
newly added surface along the spot weld projection direction. The new
node-to-surface contact pair contains the new spot weld node as a single contact
node in the pair, and surface nodes within the range of the search radius
(SHRD) specified on the SWADD
command. The search radius defaults to 4 times the spot weld radius
(SWRD) defined for the basic spot weld set. Each new
contact pair will create 6 force-distributed constraint equations internally. A new
beam is created to link the new surface to the closest existing surface through the
spot weld nodes.
After all spot weld nodes are created, the nodes of the beam elements may be reordered to link every two adjacent spot weld nodes (see Figure below). The ordering is important for the output, which is calculated for each beam in a spot weld set.
Assuming the basic spot weld set is named SWELD, below is an example of commands that could have produced the above figure.
SWADD,SWELD, ,3 ! Add Area 3 to spot weld set SWELD SWADD,SWELD, ,4 ! Add Area 4 (between surfaces 2 and 3) to SWELD
Initially, when spot weld surface 3 was added, a beam was created between surfaces 2 and 3. When surface 4 was added between surfaces 2 and 3, the beam that went between surfaces 2 and 3 was redefined to go between surfaces 2 and 4, and a new beam was created to link surfaces 4 and 3.
You can add more surfaces by repeating the SWADD command. However, the maximum number of allowable surfaces for each spot weld set (including the two surfaces used for the basic set) is 11.