4.42 PLANE42 2-D Structural Solid

An option is available to suppress the extra displacement shapes. See Section 14.42 of the ANSYS Theory Reference for more details about this element. A multi-node version of this element (PLANE82) is described in Section 4.82. An axisymmetric version that accepts nonaxisymmetric loading (PLANE25) is described in Section 4.25.

Figure 4.42-1 PLANE42 2-D Structural Solid

4.42.1 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 4.42-1. 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 pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

The nodal forces, if any, should be input per unit of depth for a plane analysis (except for KEYOPT(3)=3) and on a full 360° basis for an axisymmetric analysis. KEYOPT(2) 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).

A summary of the element input is given in Table 4.42-1. A general description of element input is given in Section 2.1.

Table 4.42-1 PLANE42 Input Summary

Element Name	PLANE42
Nodes	I, J, K, L
Degrees of Freedom	UX, UY
Real Constants	None, if KEYOPT (3) = 0, 1, 2 Thickness, if KEYOPT (3) = 3
Material Properties	EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY,ALPZ, DENS, GXY, DAMP
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 ) Fluences: FL ( I ), F L( J ), FL ( K ), FL ( L )
Special Features	Plasticity, Creep, Swelling, Stress stiffening, Large deflection, Large strain, Birth and death, Adaptive descent
KEYOPT(1)	0 - Element coordinate system is parallel to the global coordinate system 1 - Element coordinate system is based on the element I-J side
KEYOPT(2)	0 - Include extra displacement shapes 1 - Suppress extra displacement shapes
KEYOPT(3)	0 - Plane stress 1 - Axisymmetric 2 - Plane strain (Z strain = 0.0) 3 - Plane stress with thickness input
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 also. 2 - Surface solution for both faces I-J and K-L also. (Surface solution available for linear materials only) 3 - Nonlinear solution at each integration point also. 4 - Surface solution for faces with nonzero pressure

4.42.2 Output Data

• nodal displacements included in the overall nodal solution
• additional element output as shown in Table 4.42-2

The element stress directions are parallel to the element coordinate system. Surface stresses are available on any face. Surface stresses on face IJ, for example, are defined parallel and perpendicular to the IJ line and along the Z axis for a plane analysis or in the hoop direction for an axisymmetric analysis. 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 4.42-2 PLANE42 Stress Output

The following notation is used in Table 4.42-2:

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 4.42-2 PLANE42 Element Output Definitions

Name	Definition	O	R
EL	Element number	Y	Y
NODES	Nodes - I, J, K, L	Y	Y
MAT	Material number	Y	Y
THICK	Average thickness	Y	Y
VOLU:	Volume	Y	Y
CENT: X, Y	Global location 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)	Y	Y
FLUEN	Fluences FL(I), FL(J), FL(K), FL(L)	Y	Y
S:INT	Stress intensity	Y	Y
S:EQV	Equivalent stress	Y	Y
EPEL: X, Y, Z, XY	Elastic strains	Y	Y
EPEL: 1, 2, 3	Principal elastic strains	Y	Y
S: X, Y, Z, XY	Stresses (SZ=0.0 for plane stress elements)	Y	Y
S: 1, 2, 3	Principal stresses	Y	Y
EPPL: X, Y, Z, XY	Plastic strains	1	1
NL:EPEQ	Equivalent plastic strain	1	1
NL:SRAT	Ratio of trial stress to stress on yield surface	1	1
NL:SEPL	Equivalent stress on stress-strain curve	1	1
NL:HPRES	Hydrostatic pressure	-	1
EPCR: X, Y, Z, XY	Creep strains	1	1
EPSW:	Swelling strain	1	1
FACE	Face label	2	Y
EPEL(PAR,PER, Z)	Surface elastic strains (parallel, perpendicular, Z or hoop)	2	Y
TEMP	Surface average temperature	2	Y
S(PAR,PER,Z)	Surface stresses (parallel, perpendicular, Z or hoop)	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 4.42-2a PLANE42 Miscellaneous Element Output

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

1. Output at each integration point, 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

Note-For axisymmetric solutions with KEYOPT(1)=0, 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 4.42-3 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 4.42-3:

Name - output quantity as defined in the Table 4.42-2

Item - predetermined Item label for ETABLE command

E - sequence number for single-valued or constant element data

I,J,K,L - sequence number for data at nodes I,J,K,L

Name	Item	E	I	J	K	L
P1	SMISC	-	2	1	-	-
P2	SMISC	-	-	4	3	-
P3	SMISC	-	-	-	6	5
P4	SMISC	-	7	-	-	8
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
FLUEN	NMISC	-	21	22	23	24
THICK	NMISC	25	-	-	-	-

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

4.42.3 Assumptions and Restrictions

A triangular element may be formed by defining duplicate K and L node numbers (see Section 2.8). The extra shapes are automatically deleted for triangular elements so that a constant strain element results. Surface stress printout is valid only if the conditions described in Section 2.2.2 are met.

4.42.4 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.