MATRIX50

MATRIX50 is a group of previously assembled
ANSYS elements that is treated as a single element. The superelement,
once generated, may be included in any ANSYS model and used in any
analysis type for which it is applicable. The superelement can greatly
decrease the cost of many analyses. Once the superelement matrices
have been formed, they are stored in a file and can be used in other
analyses the same way any other ANSYS elements are used. Multiple
load vectors may also be stored with the superelement matrices, thereby
allowing various loading options. See MATRIX50 in the *Mechanical APDL Theory Reference* for more
details about this element.

The superelement, which is a mathematical matrix representation of an arbitrary structure, has no fixed geometrical identity and is conceptually shown in Figure 50.1. Any analysis using a superelement as one of its element types is called a superelement use pass (or run). The degrees of freedom are the master degrees of freedom specified during the generation pass.

The element name is MATRIX50 (the number 50 or the name MATRIX50 should
be input for the variable ENAME on the **ET** command). The **SE** command is used to define a superelement. **SE** reads
the superelement from Jobname.SUB (defaults to File.SUB) in the working directory. The material number
[**MAT**] is only used when material dependent damping
[**MP**,BETD] or electrical permittivity [**MP**,PERX] is an input. The real constant table number [**REAL**] is not used. However, the appropriate element type
number [**TYPE**] must be entered.

An element load vector is generated along with the element at
each load step of the superelement generation pass. Up to 31 load
vectors may be generated. Load vectors may be proportionately scaled
in the use pass. The scale factor is input on the element surface
load command [**SFE**]. The load label is input as
SELV, the load key is the load vector number, *KVAL* determines whether the load vector is real or imaginary, and the
load value is the scale factor. The load vector number is determined
from the load step number associated with the superelement generation.
If a superelement load vector has a zero scale factor (or is not
scaled at all), this load vector is not included in the analysis.
Any number of load vector-scale factor combinations may be used in
the use pass.

In a large rotation analysis (**NLGEOM**,ON),
you can use KEYOPT(3) to specify whether the load vectors associated
with this element type rotates with the element (as you would for
a pressure load) or remains in the original (unrotated) direction
(as you would for a non-follower force load); all load vectors (if
multiple load vectors) are rotated or left unrotated. You can use
KEYOPT(4) to indicate that the superelement was generated with constraints
(**D**) so that it cannot translate or rotate freely
in the use pass as expected (although you can apply constraints in
the use pass to the master degrees of freedom to prevent such motion.)

The KEYOPT(1) option is for the special case where the superelement
is to be used with a T^{4} nonlinearity, such
as for radiation. The File.SUB for this case
may be constructed directly by the user or may be generated by AUX12,
the radiation matrix generator.

A summary of the element input is given in "MATRIX50 Input Summary". A general description of element input is given in Element Input.

**Nodes**None input (supplied by element)

**Degrees of Freedom**As determined from the included element types (a mixture of multi-field degrees of freedom is not allowed)

**Real Constants**None

**Material Properties**ALPD, BETD, PERX

**Surface Loads**Surface load effects may be applied through a generated load vector and scale factors. Use the

**SFE**command to supply scale factors with LAB = SELV, LKEY = load vector number (31 maximum),*KVAL*= real or imaginary, and VAL1 = scale factor.**Body Loads**Body loads may be applied through a generated load vector and scale factors as described for surface loads.

**Special Features**Large rotation Radiation (if KEYOPT(1) = 1) **KEYOPT(1)**Element behavior:

**0 --**Normal substructure

**1 --**Special radiation substructure

**KEYOPT(3)**Load vector update with large rotations (

**NLGEOM**,ON):**0 --**Load vector(s) rotate with the substructure as it rotates

**1 --**Load vector(s) do not rotate and remain in their original direction

**KEYOPT(4)**Constrained substructure with large rotations (

**NLGEOM**,ON):**0 --**Substructure was unconstrained in the generation pass

**1 --**Substructure was constrained in the generation pass

**KEYOPT(6)**Nodal force output:

**0 --**Do not print nodal forces

**1 --**Print nodal forces

Displacements and forces may be printed for each (master) degree of freedom in a structural superelement in the "use" pass. Energies are also available when requested. The nodal forces may be output if KEYOPT(6) = 1. The stress distribution within the superelement and the expanded nodal displacements can be obtained from a subsequent stress pass. In addition to the database and substructure files from the generation run, File.DSUB must be saved from the superelement "use" pass and input to the expansion pass (if an expansion pass is desired). A general description of solution output is given in Solution Output.

A superelement may contain elements of any type except Lagrange multiplier-based elements (such as MPC184, PLANE182 with KEYOPT(6) = 1, and CONTA171 with KEYOPT(2) = 3).

See the

**D**command for degree of freedom field groups.Superelements of different field types may be mixed within the use run.

The nonlinear portion of any element included in a superelement will be ignored and any bilinear element will maintain its initial status throughout the analysis.

Superelements may contain other superelements.

The relative locations of the superelement attachment points in the nonsuperelement portion of the model (if any) should match the initial superelement geometry.

If the superelement contains a mass matrix, acceleration [

**ACEL**] defined in the use run will be applied to the superelement.If a load vector containing acceleration effects is also applied in the use run, both accelerations (the

**ACEL**command and the load vector) will be applied to the superelement.Similarly, if the superelement contains a damping matrix (as specified in the generation run) and α and β damping multipliers [

**ALPHA**and**BETA**] are defined in the use run, additional damping effects will be applied to the superelement.You should be careful to avoid duplicating acceleration and damping effects.

Pressure and thermal effects may be included in a superelement only through its load vectors.

The dimensionality of the superelement corresponds to the maximum dimensionality of any element used in its generation. A 2-D superelement should only be used in 2-D analyses, and 3-D superelements in 3-D analyses.

See Substructuring Analysis in the

*Mechanical APDL Theory Reference*for a discussion of the substructure matrix procedure.

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 Structural. **

KEYOPT(1) = 0

The PERX material property is not applicable.

**ANSYS Professional. **

This element may be used as a radiation substructure only. KEYOPT(1) defaults to 1 instead of 0 and cannot be changed.

The BETD material property, PERX material property, surface loads, and body loads are not applicable.

The large rotation special feature is not applicable.

**ANSYS Emag. **

The BETD material property is not applicable.

The large rotation special feature is not applicable.