General Axisymmetric Solid with 4 Base Nodes

Compatible Products: – | – | Premium | Enterprise | Ent PP | Ent Solver | –

SOLID272 Element Description

Use SOLID272 to model axisymmetric solid structures. It is defined by four nodes on the master plane, and nodes created automatically in the circumferential direction based on the four master plane nodes. The total number of nodes depends on the number of nodal planes (KEYOPT(2)). Each node has three degrees of freedom: translations in the nodal x, y and z directions. The element allows a triangle as the degenerated shape on the base plane to simulate irregular areas. The element has plasticity, hyperelasticity, stress stiffening, large deflection, and large strain capabilities. It also has mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and nearly and fully incompressible hyperelastic materials.

For more details about this element, see SOLID272 in the Mechanical APDL Theory Reference, and General Axisymmetric Elements in this document.

Figure 272.1:  SOLID272 Geometry (KEYOPT(2) = 3)

SOLID272 Geometry (KEYOPT(2) = 3)

SOLID272 Input Data

The geometry and node locations for this element (when KEYOPT(2) = 3) are shown in Figure 272.1: SOLID272 Geometry (KEYOPT(2) = 3). The element input data includes nodes and the orthotropic material properties. The total number of nodes is the four base nodes times the number of nodal planes. (For information about how Fourier nodes are generated, see the NAXIS command documentation.) The default element coordinate system is the cylindrical coordinate system with the z axis as the axisymmetric axis (defined via the SECDATA command) and the circumferential direction as θ. (See General Axisymmetric Elements for details.) Use the ESYS command to define an element coordinate system, which forms the basis for orthotropic material directions.

Element loads are described in Nodal Loading. Pressures must be input as element surface loads on the element edges of the nodal planes as shown by the circled numbers in Figure 272.1: SOLID272 Geometry (KEYOPT(2) = 3). Positive pressures act into the element and the maximum face edge is 4n, where n is the number of nodal planes. If pressure is applied on the element edge with face numbers less than or equal to 4 and no load on other edges, the pressure loads are the same on the 360 degrees of circumferential surfaces. (If pressure is applied on a single element edge with a face number greater than 4, the pressure is ignored.) If pressure is applied on the element edges with faces p and 4q+p (where q = 1 . . . n-1), the pressure changes linearly with respect to θ within the part of the surface bounded by the edges p and 4q+p; on the rest of the surface, the pressure is zero.

Temperatures may be input as element body loads at the nodes. For the four nodes on the master plane, the node I1 temperature T(I1) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I1). For any other input pattern, unspecified temperatures default to TUNIF. For the nodes generated in the circumferential direction based on the master node, they default to the value of their base nodes (T(I1), T(J1), T(K1) or T(L1), depending on their location) if all other temperatures are unspecified. For any other input pattern, unspecified temperatures default to TUNIF.

KEYOPT(6) = 1 sets the element for using mixed formulation. For details on the use of mixed formulation, see Applications of Mixed u-P Formulations in this document.

As described in Coordinate Systems, you can use the ESYS command to orient the material properties and strain/stress output. Use RSYS to choose output that follows the material coordinate system or the global coordinate system.

The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, issue a NROPT,UNSYM command. For a geometric nonlinear analysis when convergence is an issue, use an unsymmetric matrix.

"SOLID272 Input Summary" contains a summary of the element input. See Element Input in this document for a general description of element input.

SOLID272 Input Summary


I1, J1, K1, L1, I2, J2, K2, L2, . . . , In, Jn, Kn, Ln (where n = KEYOPT(2), the number of nodal planes)

Degrees of Freedom


Real Constants
Material Properties

TB command: See Element Support for Material Models for this element.




Surface Loads
Pressures -- 

edge 1 (J1-I1), edge 2 (K1-J1), edge 3 (L1-K1), edge 4 (I1-L1), edge 5 (J2-I2), edge 6 (K2-J2), . . . , edge 4n-3(Jn-In), edge 4n-2 (Kn-Jn), edge 4n-1 (Ln-Kn), edge 4n (In-Ln)

Body Loads
Temperatures -- 

T(I1), T(J1), T(K1), T(L1), T(I2), T(J2), T(K2), T(L2), . . . , T(In), T(Jn), T(Kn), T(Ln)

Special Features
Birth and death
Coriolis effect
Element technology autoselect
Large deflection
Large strain
Nonlinear stabilization
Stress stiffening

Number of Fourier nodes in the circumferential direction (that is, the number of nodal planes):

1 -- 

Axisymmetric deformation (may have torsion)

3 - 12 -- 

General 3-D deformation

This KEYOPT has no default. You must specify a valid value. (0 is not valid.)

For large-rotation not about the axisymmetric axis, KEYOPT(2) 5 is recommended.

For information about specifying the number of Fourier nodes, see General Axisymmetric Elements in this document.

For information about how Fourier nodes are generated, see the NAXIS command documentation.


Element formulation:

0 -- 

Use pure displacement formulation (default)

1 -- 

Use mixed u-P formulation

SOLID272 Output Data

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

As shown in Figure 272.2: SOLID272 Stress Output, the element stress directions are parallel to the element coordinate system. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

To view 3-D mode shapes for a modal or eigenvalue buckling analysis, expand the modes with element results calculation active (via the MXPAND command's Elcalc = YES option).

Figure 272.2:  SOLID272 Stress Output

SOLID272 Stress Output

Element stress directions SX, SY, and SZ shown in the global coordinate system.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 272.1:  SOLID272 Element Output Definitions

Name Definition O R
ELElement number-Y
NODESNodes - I1, J1, K1, L1, I2, J2, K2, L2, . . .-Y
MATMaterial number-Y
XC, YC, ZCLocation where results are reported- 3

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

See Table 272.2: SOLID272 Item and Sequence Numbers for more output.

TEMPTemperatures T(I1), T(J1), T(K1), T(L1), T(I2), T(J2), T(K2), T(L2), . . . -Y
S:X, Y, Z, XY, YZ, XZStressesYY
S:1, 2, 3Principal stresses-Y
S:INTStress intensity-Y
S:EQVEquivalent stressYY
EPEL:X, Y, Z, XY, YZ, XZElastic strainsYY
EPEL:1, 2, 3Principal elastic strains-Y
EPEL:EQVEquivalent elastic strain [6]YY
EPTH:X, Y, Z, XY, YZ, XZThermal strains 2 2
EPTH:EQVEquivalent thermal strain [6] 2 2
EPPL:X, Y, Z, XY, YZ, XZPlastic strains[7] 1 1
EPPL:EQVEquivalent plastic strain [6] 1 1
EPCR:X, Y, Z, XY, YZ, XZCreep strains 1 1
EPCR:EQVEquivalent creep strains [6] 1 1
EPTO:X, Y, Z, XY, YZ, XZTotal mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)Y-
NL:EPEQAccumulated equivalent plastic strain 1 1
NL:CREQAccumulated equivalent plastic strain 1 1
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding) 1 1
NL:PLWKPlastic work/volume 1 1
NL:HPRESHydrostatic pressure 1 1
SEND:ELASTIC, PLASTIC, CREEP, ENTOStrain energy densities- 1
LOCI:X, Y, ZIntegration point locations- 4
SVAR:1, 2, . . . , NState variables- 5

  1. Nonlinear solution, output only if the element has a nonlinear material.

  2. Output only if element has a thermal load.

  3. Available only at centroid as a *GET item.

  4. Available only if OUTRES,LOCI is used.

  5. Available only if the UserMat subroutine and TB,STATE command are used.

  6. The equivalent strains use an effective Poisson's ratio: for elastic and thermal strains, this value must be specified (MP,PRXY); for plastic and creep strains, this value is set at 0.5.

  7. For the shape memory alloy material model, transformation strains are reported as plasticity strain EPPL.

Table 272.2: SOLID272 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The following notation is used in the output table:


output quantity as defined in the Table 272.1: SOLID272 Element Output Definitions


predetermined Item label for ETABLE

I1, J1, K1, L1, I2, J2, K2, L2, . . .

sequence number for data at nodes I1, J1, K1, L1, I2, J2, K2, L2, . . .

Table 272.2:  SOLID272 Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input
Item I1 J1 K1 L1 I2 J2 K2 L2 --- In Jn Kn Ln
P1 SMISC21 ---
P2 SMISC 43 ---
P3 SMISC 65 ---
P4 SMISC7 8 ---
P5 SMISC 109 ---
P6 SMISC 1211 ---
P7 SMISC 1413---
P8 SMISC 15 16---
--- ------------------------------------------
P4n-3 SMISC ---8n-68n-7
P4n-2 SMISC --- 8n-48n-5
P4n-1 SMISC --- 8n-28n-3
P4n SMISC ---8n-1 8n

SOLID272 Assumptions and Restrictions

  • The area of the base element must be nonzero.

  • The base element must lie on one side of the axisymmetric axis, and the axisymmetric axis must be on the same plane as the base element (master plane).

  • A base element or base node must be associated with one axisymmetric axis (defined via SECTYPE and SECDATA commands) before generating nodes for general axisymmetric element sections (NAXIS) or defining an element by node connectivity (E).

  • You can form a triangular base element by defining duplicate K1 and L1 node numbers. (See Degenerated Shape Elements in this document.)

  • You cannot apply a pressure load via the SFA command.

  • Incompressible and nearly incompressible material behavior should be modeled with the mixed u-P formulation.

  • If you specify mixed formulation (KEYOPT(6) = 1), you must use the sparse solver.

  • The contribution of the element to the mass moment inertia of the whole model is calculated by element mass multiplied by the square of the coordinates of the elemental centroid. The moment of inertia may therefore be inaccurate.

  • The element does not support the expansion pass of a superelement with large rotation.

  • Issuing an /ESHAPE,1 command while PowerGraphics is active causes the program to plot the elements in 3-D and the results on both nodal planes and all integration planes in the circumferential direction; otherwise, the program plots the elements in 2-D and the results on the master plane.

  • You cannot display surface load symbols (/PSF) when displaying this element in 3-D via the /ESHAPE command.

  • When specifying more than one facet per element edge for PowerGraphics displays (NAXIS,EFACET,NUM, where NUM > 1), ANSYS plots additional results on some planes between the nodal and integration planes. The results on these planes are interpolated based on the nodal and integration plane values and are therefore less accurate than the values on the nodal and interpolation planes. If you do not wish to plot the interpolated values, set NUM = 1 to plot only the values on nodal and integration planes.

  • Print commands in postprocessing print the nodal plane results only.

  • To model axisymmetric solid surface loads acting on this element, use general axisymmetric surface element SURF159. (You cannot use this element with surface-effect elements SURF153 and SURF154.)

  • You cannot generate surface-based contact pairs (contact elements CONTA171 through CONTA174 paired with target elements TARGE169 and TARGE170) on this element.

  • You can generate node-to-surface contact pairs (contact elements CONTA175 paired with target elements TARGE170) and node-to-node contact elements (CONTA178) on this element, with the following restrictions:

    • When TARGE170 is on the surface of SOLID272, you may have accuracy and convergence issues if the loading causes large rotations about the axisymmetric axis of SOLID272; you may also have those issues if the two sides of the contact boundaries have different mesh patterns in the circumferential direction (caused by different KEYOPT(2) values of SOLID272).

    • You cannot define CONTA175 with the multipoint constraint (MPC) approach using a force-distributed constraint (that is, you cannot set KEYOPT(2) = 2, KEYOPT(4) = 1, and KEYOPT(12) = 5 or 6 simultaneously for the CONTA175 elements).

    • In the case of a true axisymmetric condition (SOLID272 with KEYOPT(2) = 1), you should use 2-D node-to-surface contact pairs (CONTA175 contact elements paired with TARGE169 target elements).

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Prestress effects can be activated via the PSTRES command.

SOLID272 Product Restrictions

There are no product-specific restrictions for this element.

Release 18.2 - © ANSYS, Inc. All rights reserved.