4.92 SOLID92 3-D 10-Node Tetrahedral Structural Solid

4.92 SOLID92 3-D 10-Node Tetrahedral Structural Solid (UP19980821 ) SOLID92 has a quadratic displacement behavior and is well suited to model irregular meshes (such as produced from various CAD/CAM systems). A 20-node brick shaped element, SOLID95, is described in Section 4.95. A 4-node tetrahedral element, SOLID72, is described in Section 4.72.

The element is defined by ten nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. The element also has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities. See Section 14.92 of the ANSYS Theory Reference for more details about this element.

Figure 4.92-1 SOLID92 3-D 10-Node Tetrahedral Structural Solid



4.92.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.92-1.

Beside the nodes, the element input data includes the orthotropic material properties. 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 4.92-1. Positive pressures act into the element. Temperatures and fluences 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. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

A summary of the element input is given in Table 4.92-1. A general description of element input is given in Section 2.1.

Table 4.92-1 SOLID92 Input Summary

Element Name

SOLID92

Nodes

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

Degrees of Freedom

UX, UY, UZ

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

Body Loads

Temperatures:
T (I), T (J), T (K), T (L), T (M), T (N), T (O), T (P), T (Q), T (R)
Fluences:
FL (I), FL (J), FL (K), FL (L), FL (M), FL (N), FL (O), FL (P),
FL (Q), F L (R)

Special Features

Plasticity, Creep, Swelling, Stress stiffening, Large deflection, Large strain, Birth and death, Adaptive descent.

KEYOPT(5)

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

KEYOPT(6)

0 - Basic element printout
4 - Surface printout for faces with nonzero pressure

4.92.2 Output Data

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

Several items are illustrated in Figure 4.92-2. The element stress directions are parallel to the element coordinate system. The surface stress outputs are in the surface coordinate system and are available for any face (KEYOPT(6)). The coordinate system for face JIK is shown in Figure 4.92-2. The other surface coordinate systems follow similar orientations as indicated by the pressure face node description. Surface stress printout is valid only if the conditions described in Section 2.2.2 are met. 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 4.92-2 SOLID92 Stress Output



The following notation is used in Table 4.92-2:

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 4.92-2 SOLID92 Element Output Definitions

Name

Definition

O

R

EL

Element number

Y Y
NODES

Corner nodes - I, J, K, L

Y Y
MAT

Material number

Y Y
VOLU:

Volume

Y Y
CENT: X, Y, Z

Global X, Y, Z location of centroid

Y Y
PRES

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

Y Y
TEMP

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

Y Y
FLUEN

Fluences FL(I), FL(J), FL(K), FL(L), FL(M), FL(N), FL(O), FL(P), FL(Q), FL(R)

Y Y
S:INT

Stress intensity

Y Y
S:EQV

Equivalent stress

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

Stresses

Y Y
S: 1, 2, 3

Principal stresses

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

Elastic strains

Y Y
EPEL: 1, 2, 3

Principal elastic strains

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

Plastic strains

1 1
EPCR: X, Y, Z, XY, YZ, XZ

Creep strains

1 1
EPSW:

Swelling strain

1 1
NL:EPEQ

Average equivalent plastic strain

1 1
NL:SRAT

Ratio of trial stress to stress on yield surface

1 1
NL:SEPL

Equivalent stress from stress-strain curve

1 1
NL:HPRES

Hydrostatic pressure

- 1
FACE

Face label

2 Y
TRI

Nodes on this face

2 -
AREA

Face area

2 Y
TEMP

Face average temperature

2 Y
EPEL(X,Y,XY)

Surface elastic strains

2 Y
PRES

Surface pressure

2 Y
S(X,Y,XY)

Surface stresses

2 Y
S(1,2,3)

Surface principal stresses

2 Y
SINT

Surface stress intensity

2 Y
SEQV

Surface equivalent stress

2 Y
1. Nonlinear solution (output if the element has a nonlinear material)

2. Face output (if KEYOPT(6)=4 and a nonzero pressure face)

Table 4.92-2a SOLID92 Miscellaneous Element Output

Description

Names of Items Output

O

R

Integration Point Stress Solution

TEMP, SINT, SEQV, EPEL, S, EPPL, EPCR,
EPSW, EPEQ, SRAT, SEPL, HPRES

1 -
Nodal Stress Solution

LOCATION, TEMP, SINT, SEQV, S

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

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

Table 4.92-3 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 4.92-3:

Table 4.92-3 SOLID92 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name

Item

I

J

K

L

M

N

O

P

Q

R

P1

SMISC

2 1 3 - - - - - - -
P2

SMISC

4 5 - 6 - - - - - -
P3

SMISC

- 7 8 9 - - - - - -
P4

SMISC

11 - 10 12 - - - - - -
See Section 2.2.2.5 of this manual for the item and sequence numbers for surface output for the ETABLE command.

4.92.3 Assumptions and Restrictions

The element must not have a zero volume. Elements may be numbered either as shown in Figure 4.92-1 or may have node L below the IJK plane. An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. See Section 2.4.2 of the ANSYS Modeling and Meshing Guide for information about the use of midside nodes.

4.92.4 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/LinearPlus