MPC184-Weld

Multipoint Constraint Element: Weld Joint

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

## MPC184 Weld Joint Element Description

The MPC184 weld joint element is a two-node element that has all relative degrees of freedom fixed.

## MPC184 Weld Joint Input Data

Set KEYOPT(1) = 13 to define a two-node weld joint element.

Figure 184weld.1: MPC184 Weld Joint Geometry shows the geometry and node locations for this element. Two nodes (I and J) define the element.

A local Cartesian coordinate system must be specified at the first node, I, of the element. The local coordinate system specification at the second node is optional. The local coordinate systems specified at node I and J evolve with the rotations at the respective nodes. Use the SECJOINT command to specify the identifiers of the local coordinate systems.

Other input data that are common to all joint elements (material behavior, etc.) are described in "Joint Input Data" in the MPC184 element description.

Note:  The weld joint may also be simulated by using the CE command. See the CE command description for additional details.

### MPC184 Weld Joint Input Summary

This input summary applies to the weld joint element option of MPC184: KEYOPT(1) = 13.

Nodes

I, J

Note:  For a grounded joint element, specify either node I or node J in the element definition and leave the other node (the grounded node) blank.

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

None

Material Properties

None

None

None

None

Special Features
 Large deflection Linear perturbation
KEYOPT(1)

Element behavior:

13  --

Weld joint element

## MPC184 Weld Joint Output Data

The solution output associated with the element is in two forms:

These tables use the following notation:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available.

Table 184weld.1:  MPC184 Weld Joint Element Output Definitions

NameDefinitionOR
ELElement number-Y
NODESElement node numbers (I, J)-Y
FXConstraint force in X direction-Y
FYConstraint force in Y direction-Y
FZConstraint force in Z direction-Y
MXConstraint moment in X direction-Y
MYConstraint moment in Y direction-Y
MZConstraint moment in Z direction-Y

The following table shows additional non-summable miscellaneous (NMISC) output available for the weld joint element.

Note:  This output is intended for use in the ANSYS Workbench program to track the evolution of local coordinate systems specified at the nodes of joint elements.

Table 184weld.2:  MPC184 Weld Joint Element - NMISC Output

NameDefinitionOR
E1X-I, E1Y-I, E1Z-IX, Y, Z components of the evolved e1 axis at node I-Y
E2X-I, E2Y-I, E2Z-IX, Y, Z components of the evolved e2 axis at node I-Y
E3X-I, E3Y-I, E3Z-IX, Y, Z components of the evolved e3 axis at node I-Y
E1X-J, E1Y-J, E1Z-JX, Y, Z components of the evolved e1 axis at node J-Y
E2X-J, E2Y-J, E2Z-JX, Y, Z components of the evolved e2 axis at node J-Y
E3X-J, E3Y-J, E3Z-JX, Y, Z components of the evolved e3 axis at node J-Y
JFX, JFY, JFZConstraint forces expressed in the evolved coordinate system specified at node I-Y
JMX, JMY, JMZConstraint moments expressed in the evolved coordinate system specified at node I-Y

Table 184weld.3: MPC184 Weld Joint Item and Sequence Numbers - SMISC Items and Table 184weld.4: MPC184 Weld Joint Item and Sequence Numbers - NMISC Items list output available via the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table for further information. The table uses the following notation:

Name

output quantity as defined in the Element Output Definitions table.

Item

predetermined Item label for ETABLE command

E

sequence number for single-valued or constant element data

Table 184weld.3:  MPC184 Weld Joint Item and Sequence Numbers - SMISC Items

Output Quantity NameETABLE and ESOL Command Input
ItemE
FXSMISC1
FYSMISC2
FZSMISC3
MXSMISC4
MYSMISC5
MZSMISC6

Table 184weld.4:  MPC184 Weld Joint Item and Sequence Numbers - NMISC Items

Output Quantity NameETABLE and ESOL Command Input
ItemE
E1X-INMISC1
E1Y-INMISC2
E1Z-INMISC3
E2X-INMISC4
E2Y-INMISC5
E2Z-INMISC6
E3X-INMISC7
E3Y-INMISC8
E3Z-INMISC9
E1X-JNMISC10
E1Y-JNMISC11
E1Z-JNMISC12
E2X-JNMISC13
E2Y-JNMISC14
E2Z-JNMISC15
E3X-JNMISC16
E3Y-JNMISC17
E3Z-JNMISC18
JFXNMISC19
JFYNMISC20
JFZNMISC21
JMXNMISC22
JMYNMISC23
JMZNMISC24

## MPC184 Weld Joint Assumptions and Restrictions

• Boundary conditions cannot be applied on the nodes forming the weld joint.

• Rotational degrees of freedom are activated at the nodes forming the element. When these elements are used in conjunction with solid elements, the rotational degrees of freedom must be suitably constrained. Since boundary conditions cannot be applied to the nodes of the weld joint, a beam or shell element with very weak stiffness may be used with the underlying solid elements at the nodes forming the joint element to avoid any rigid body modes.

• Stops (SECSTOP) and locks (SECLOCK) are not applicable to this element.

• In a nonlinear analysis, the components of relative motion are accumulated over all the substeps. It is essential that the substep size be restricted such that these rotations in a given substep are less than π for the values to be accumulated correctly.

• The element currently does not support birth or death options.

• The equation solver (EQSLV) must be the sparse solver or the PCG solver. The command PCGOPT,,,,,,,ON is also required in order to use the PCG solver.

• The element coordinate system (/PSYMB,ESYS) is not relevant.

## MPC184 Weld Joint Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro

• Linear perturbation is not available.