4.73 SOLID73 3-D 8-Node Structural Solid with Rotations

4.73 SOLID73 3-D 8-Node Structural Solid with Rotations (UP19980821 ) SOLID73 is used for the three-dimensional modeling of solid structures. The element is defined by eight nodes having six degrees of freedom at each node: translations in the nodal x, y, and z directions and rotations about the nodal x, y, and z axes. A similar 4-node tetrahedron element (SOLID72) is described in Section 4.72. A 20-node solid without rotational degrees of freedom (SOLID95) is described in Section 4.95.

The SOLID73 element can often be used in place of the SOLID95 element to reduce the wavefront and solution time (since it does not have midside nodes). Although the element has additional degrees of freedom per node, it is not quite as accurate as the SOLID95 element. See Section 14.73 of the ANSYS Theory Reference for more details about this element.

Figure 4.73-1 SOLID73 3-D 8-Node Structural Solid with Rotations



4.73.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.73-1. The element is defined by eight nodes and the orthotropic material properties. A tetrahedral-shaped element may be formed by defining the same node numbers for nodes M, N, O, and P; and nodes K and L. A wedge-shaped element and a pyramid-shaped element may also be formed as shown in Figure 4.73-1. Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Section 2.3. Properties not input default as described in Section 2.4.

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 4.73-1. 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). For any other input pattern, unspecified temperatures default to TUNIF.

A summary of the element input is given in Table 4.73-1. A general description of element input is given in Section 2.1.

Table 4.73-1 SOLID73 Input Summary

Element Name

SOLID73

Nodes

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

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

None

Material Properties

EX, EY, EZ, ALPX, ALPY, ALPZ, (PRXY, PRYZ, PRXZ
or NUXY, NUYZ, NUXZ), DENS, GXY, GYZ, GXZ, DAMP

Surface Loads

Pressures:
face 1 (J-I-L-K), face 2 (I-J-N-M), face 3 (J-K-O-N),
face 4 (K-L-P-O), face 5 (L-I-M-P), face 6 (M-N-O-P)

Body Loads

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

Special Features

Stress stiffening, Birth and death

KEYOPT(5)

0 - Basic element printout
1 - Integration point printout
2 - Nodal stress printout

4.73.2 Output Data

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

Several items are illustrated in Figure 4.73-2. The element stress directions are parallel to the element 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 4.73-2 SOLID73 Stress Output



The following notation is used in Table 4.73-2:

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 4.73-2 SOLID73 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, Z

Global location XC, YC, ZC

Y Y
PRES

Pressures P1 at nodes J, I, L, K; P2 at I, J, N, M; P3 at J, K, O, N;
P4 at K, L, P, O; P5 at L, I, M, P; P6 at M, N, O, P

Y Y
TEMP

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

Y Y
S:INT

Stress intensity

Y Y
S:EQV

Equivalent stress

Y Y
EPEL: X, Y, Z, XY, YZ, XZ

Elastic strains

Y Y
EPEL: 1, 2, 3

Principal elastic strains

Y Y
S: X, Y, Z, XY, YZ, XZ

Stresses

Y Y
S: 1, 2, 3

Principal stresses

Y Y
Table 4.73-2a SOLID73 Miscellaneous Element Output

Description

Names of Items Output

O

R

Integration Point Stress Solution

X, Y, Z, TEMP, SINT, SEQV, EPEL, S

1 -
Nodal Stress Solution

TEMP, S, SINT, SEQV

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

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

Table 4.73-3 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 4.73-3:

Table 4.73-3 SOLID73 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

I

J

K

L

M

N

O

P

P1

SMISC

2 1 4 3 - - - -
P2

SMISC

5 6 - - 8 7 - -
P3

SMISC

- 9 10 - - 12 11 -
P4

SMISC

- - 13 14 - - 16 15
P5

SMISC

18 - - 17 19 - - 20
P6

SMISC

- - - - 21 22 23 24
S:1

NMISC

1 6 11 16 21 26 31 36
S:2

NMISC

2 7 12 17 22 27 32 37
S:3

NMISC

3 8 13 18 23 28 33 38
S:INT

NMISC

4 9 14 19 24 29 34 39
S:EQV

NMISC

5 10 15 20 25 30 35 40

4.73.3 Assumptions and Restrictions

Zero volume elements are not allowed. Elements may be numbered either as shown in Figure 4.73-1 or may have the planes IJKL and MNOP interchanged. The element may not be twisted such that it has two separate volumes. This occurs most frequently when the elements are not numbered properly. All elements must have eight nodes.

Care should be taken when applying force loads and displacement constraints to this solid element with rotational degrees of freedom. For uniform results, applied moments should accompany applied forces and rotational displacement constraints should be applied where appropriate. The rotational stiffness of an isolated node or line of nodes is quite small and is typically inappropriate as the sole rotational constraint of the model or an adjacent beam or shell element. Applied pressure loads on an element face are automatically converted to the equivalent force and moment loads. Due to a theoretical limitation, you may not use SURF22 to apply pressure loads to SOLID73. When the SOLID73 elements are used with other element types, the constraints to prevent rigid body motion should be specified on the nodes of the SOLID73 elements. It is also recommended that at least one of the nodes have specified constraints in each of the three rotational directions. For reduced analyses, rotational degrees of freedom should not be selected as master degrees of freedom (also suppressed during automatic [TOTAL] master degree of freedom selection).

Degeneration to the form of pyramid should be used with caution. The element sizes, when degenerated, should be small in order to minimize the stress gradients. Pyramid elements are best used as filler elements or in meshing transition zones.

4.73.4 Product Restrictions

ANSYS/LinearPlus