4.45 SOLID45 3-D Structural Solid

The element has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities. A reduced integration option with hourglass control is available. See Section 14.45 of the ANSYS Theory Reference for more details about this element. A similar element with anisotropic properties (SOLID64) is described in Section 4.64. A higher-order version of the SOLID45 element (SOLID95) is described in Section 4.95.

Figure 4.45-1 SOLID45 3-D Structural Solid

4.45.1 Input Data

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 4.45-1. 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). For any other input temperature pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

KEYOPT(1) is used to include or suppress the extra displacement shapes. KEYOPT(5) and KEYOPT(6) provide various element printout options (see Section 2.2.2).

This element also supports uniform reduced (1 point) integration with hourglass control when KEYOPT(2)=1. Using uniform reduced integration provides the following advantages when running a nonlinear analysis:

• Less CPU time is required for element stiffness formation and stress/strain calculations to achieve a comparable accuracy to the FULL integration option.
• The length of the element history saved record (*.ESAV and *.OSAV) is about 1/7th as much as when the full integration (2 X 2 X 2) is used for the same number of elements.
• Nonlinear convergence characteristic of the option is generally far superior to the default full integration with extra displacement shape, i.e. KEYOPT(1)=0, KEYOPT(2)=0.
• The analysis will not suffer from volumetric locking which can be caused by plasticity or other incompressible material properties.

• The analysis is not as accurate as the full integration method, which is apparent in the linear analysis for the same mesh.
• The analysis cannot capture the bending behavior with a single layer of elements, for example, in the case of a fixed-end cantilever with a lateral point load, modeled by one layer of elements laterally. Instead, four elements are usually recommended.

the solution is generally acceptable. If the ratio exceeds 5%, refine the mesh. The total energy and artificial energy can also be monitored by using the OUTPR, VENG command in the solution phase.

A summary of the element input is given in Table 4.45-1. A general description of element input is given in Section 2.1.

Table 4.45-1 SOLID45 Input Summary

Element Name	SOLID45
Nodes	I, J, K, L, M, N, O, P
Degrees of Freedom	UX, UY, UZ
Real Constants	Hourglass control factor needed only when KEYOPT(2)=1. Note-The valid value for this real constant is any positive number; default=1.0. We recommend that you use a value between 1 and 10.
Material Properties	EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ, 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 ) Fluences: FL ( I ), F L( J ), FL ( K ), FL ( L ), FL ( M ), FL ( N ), FL ( O ), FL ( P )
Special Features	Plasticity, Creep, Swelling, Stress stiffening, Large deflection, Large strain, Birth and death, Adaptive descent
KEYOPT(1)	0 - Include extra displacement shapes 1 - Suppress extra displacement shapes
KEYOPT(2)	0 - Full integration with or without extra displacement shapes, depending on the setting of KEYOPT(1) 1 - Uniform reduced integration with hourglass control; suppress extra displacement shapes (KEYOPT(1) is automatically set to 1.).
KEYOPT(4)	0 - Element coordinate system is parallel to the global coordinate system 1 - Element coordinate system is based on the element I-J side
KEYOPT(5)	0 - Basic element solution 1 - Repeat basic solution for all integration points 2 - Nodal stress solution
KEYOPT(6)	0 - Basic element solution 1 - Surface solution for face I-J-N-M also 2 - Surface solution for face I-J-N-M and face K-L-P-O (Surface solution available for linear materials only) 3 - Nonlinear solution at each integration point also 4 - Surface solution for faces with nonzero pressure

4.45.2 Output Data

• nodal displacements included in the overall nodal solution
• additional element output as shown in Table 4.45-2

Figure 4.45-2 SOLID45 Stress Output

When KEYOPT(2)=1 (the element is using uniform reduced integration), all the outputs for the element integration points are output in the same style as the full integration outputs. The number of points for full integration is used for consistency of output within the same element type.

The following notation is used in Table 4.45-2:

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 4.45-2 SOLID45 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
FLUEN	Fluences FL(I), FL(J), FL(K), FL(L), FL(M), FL(N), FL(O), FL(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
EPPL: X, Y, Z, XY, YZ, XZ	Average plastic strains	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	Average equivalent stress from stress-strain curve	1	1
NL:HPRES	Hydrostatic pressure		1
EPCR: X, Y, Z, XY, YZ, XZ	Average creep strains	1	1
EPSW:	Average swelling strain	1	1
FACE	Face label	2	Y
AREA	Face area	2	Y
TEMP	Surface average temperature	2	Y
EPEL	Surface elastic strains (X,Y,XY)	2	Y
PRESS	Surface pressure	2	Y
S(X, Y, XY)	Surface stresses (X axis parallel to line defined by first two nodes which define the face)	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 only if the element has a nonlinear material

2. Face printout (if KEYOPT(6) is 1,2, or 4)

Table 4.45-2a SOLID45 Miscellaneous Element Output

Description	Names of Items Output	O	R
Nonlinear Integration Pt. Solution	EPPL, EPEQ, SRAT, SEPL, HPRES, EPCR, EPSW	1	-
Integration Point Stress Solution	TEMP, S(X, Y, Z, XY, YZ, XZ), SINT, SEQV, EPEL	2	-
Nodal Stress Solution	TEMP, S(X, Y, Z, XY, YZ, XZ), SINT, SEQV, EPEL	3	-

1. Output at each of eight integration points, if the element has a nonlinear material and KEYOPT(6)=3

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

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

Table 4.45-3 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 4.45-3:

Name - output quantity as defined in the Table 4.45-2

Item - predetermined Item label for ETABLE command

I,J,...,P - sequence number for data at nodes I,J,...,P

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
FLUEN	NMISC	41	42	43	44	45	46	47	48

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

4.45.3 Assumptions and Restrictions

All elements must have eight nodes. A prism-shaped element may be formed by defining duplicate K and L and duplicate O and P node numbers (see Section 2.8). A tetrahedron shape is also available. The extra shapes are automatically deleted for tetrahedron elements.

4.45.4 Product Restrictions

ANSYS/LinearPlus

• The DAMP material property is not allowed.
• Fluence body loads are not applicable.
• The only special feature allowed is stress stiffening.
• KEYOPT(6)=3 is not applicable.