4.88 VISCO88 2-D 8-Node Viscoelastic Solid

4.88 VISCO88 2-D 8-Node Viscoelastic Solid (UP19980821 ) VISCO88 is a quadratic isoparametric element. The element is defined by eight nodes having two degrees of freedom at each node: translations in the nodal x and y directions. The element may be used as a plane strain or as an axisymmetric element. The element has viscoelastic and stress stiffening capabilities. Various printout options are also available.

Figure 4.88-1 VISCO88 2-D 8-Node Viscoelastic Solid



4.88.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.88-1. The element coordinate system orientation is as described in Section 2.3.

A triangular-shaped element may be formed by defining the same node number for nodes K, L and O. Details of the required material properties are provided in Section 2.5.3.

Element loads are described in Section 2.7. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 4.88-1. Positive pressures act into the element. Temperatures may be input as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). If all corner node temperatures are specified, each midside node temperature defaults to the average temperature of its adjacent corner nodes. For any other input temperature pattern, unspecified temperatures default to TUNIF.

The nodal forces, if any, should be input per unit of depth for a plane analysis and on a full 360° basis for an axisymmetric analysis. KEYOPT(5) provides various element printout options (see Section 2.2.2).

A summary of the element input is given in Table 4.88-1. A general description of element input is given in Section 2.1.

Table 4.88-1 VISCO88 Input Summary

Element Name

VISCO88

Nodes

I, J, K, L, M, N, O, P

Degrees of Freedom

UX, UY

Real Constants

None

Material Properties

DENS (see Section 2.5.3 for others)

Surface Loads

Pressures:
face 1 (J-I), face 2 (K-J), face 3 (L-K), face 4 (I-L)

Body Loads

Temperatures:
T (I), T (J), T (K), T (L), T (M), T (N), T (O), T (P)

Special Features

Viscoelasticity, Stress stiffening

KEYOPT(3)

0, 2 Plane strain (Z strain = 0.0)
1 - Axisymmetric

KEYOPT(5)

0 - Basic element printout
1 - Repeat basic element printout for all integration points
2 - Nodal stress printout

4.88.2 Output Data

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

The element stress directions are shown in Figure 4.88-2. The directions are parallel to the global Cartesian coordinate system. A general description of solution output is given in Section 2.2. See the ANSYS Basic Analysis Procedures Guide for ways to view results.

Figure 4.88-2 VISCO88 Stress Output



The following notation is used in Table 4.88-2:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). The O and R columns indicate the availability of the items in the file Jobname.OUT (O) or in the results file (R), a Y indicates that the item is always available, a number refers to a table footnote which describes when the item is conditionally available, and a - indicates that the item is not available.

Table 4.88-2 VISCO88 Element Output Definitions

Name

Definition

O

R

EL

Element number

Y Y
NODES

Nodes - I, J, K, L, M, N, O, P

Y Y
MAT

Material number

Y Y
VOLU:

Volume

Y Y
CENT: X, Y

Global location of centroid XC, YC

Y Y
PRES

Pressures P1 at nodes J,I; P2 at K,J; P3 at L,K; P4 at I,L

Y Y
TEMP

Temperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)

Y Y
S: X, Y, Z, XY

Stresses (See Note 2.)

Y Y
S: 1, 2, 3

Principal stresses

Y Y
S:INT

Stress intensity

Y Y
S:EQV

Equivalent stress

Y Y
GR STRAIN

Growth strain (recoverable and irrecoverable thermally induced effects)

Y Y
FICT TEMP

Fictive or pseudo temperature

Y Y
EFF BULK MOD

Effective bulk modulus

1 1
EFF SHEAR MOD

Effective shear modulus

1 1
1. Element solution output quantities EFF BULK MOD and EFF SHEAR MOD might not correspond to the effective bulk and shear moduli, respectively. The output values are actually intermediate quantities in the computation of bulk and shear moduli and do not represent any true tangible material properties. These quantities are also stored on the results files as nonsummable miscellaneous (NMISC) data items 25 through 32 (ETABLE command).

Table 4.88-2a VISCO88 Miscellaneous Element Output

Description

Names of Items Output

O

R

Integration Point Solution

S(X, Y, Z, XY, YZ, XZ), S(1, 2, 3), SINT, SEQV,
GR STRAIN, FICT TEMP, EFF BULK MOD,
EFF SHEAR MOD

1 -
Nodal Stress Solution

TEMP, S(X, Y, Z, XY), SINT, SEQV

2 -
1. Output at each integration point, if KEYOPT(5)=1

2. Output at each node, if KEYOPT(5)=2

Note 1. Displacements and nodal forces are the total (not incremental) values.

Note 2. For axisymmetric solutions, the X,Y,Z and XY stress and strain outputs correspond to the radial, axial, hoop, and in-plane shear stresses and strains, respectively.

Table 4.88-3 lists output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide and Section 2.2.2.2 of this manual for more information. The following notation is used in Table 4.88-3:

Table 4.88-3 VISCO88 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

I

J

K

L

S:1

NMISC

1 6 11 16
S:2

NMISC

2 7 12 17
S:3

NMISC

3 8 13 18
S:INT

NMISC

4 9 14 19
S:EQV

NMISC

5 10 15 20
FICT TEMP

NMISC

21 22 23 24
EFF BULK MOD

NMISC

25 26 27 28
EFF SHEAR MOD

NMISC

29 30 31 32
GR STRAIN

NMISC

33 34 35 36

4.88.3 Assumptions and Restrictions

The area of the element must be positive. The element must lie in a global X-Y plane as shown in Figure 4.88-1 and the Y-axis must be the axis of symmetry for axisymmetric analyses. An axisymmetric structure should be modeled in the +X quadrants. A face with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that face. See Section 2.4.2 of the ANSYS Modeling and Meshing Guide for more information about the use of midside nodes.

4.88.4 Product Restrictions

There are no product-specific restrictions for this element.