3-D Reinforced Concrete Solid

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

SOLID65 Element Description

Although this legacy element is available for use in your analysis, ANSYS, Inc. recommends using the current-technology element SOLID185, specifying either full integration with the method (KEYOPT(3) = 0 and KEYOPT(2) = 3), or simplified enhanced strain formulation (KEYOPT(3) = 0 and KEYOPT(2) = 0). For more information, see Microplane in the Material Reference.

SOLID65 is used for 3-D modeling of solids with or without reinforcing bars (rebar). The solid is capable of cracking in tension and crushing in compression. In concrete applications, for example, the solid capability of the element may be used to model the concrete while the rebar capability is available for modeling reinforcement behavior. Other cases for which the element is also applicable would be reinforced composites (such as fiberglass), and geological materials (such as rock). The element is defined by eight nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. Up to three different rebar specifications may be defined.

The concrete element is similar to a 3-D structural solid but with the addition of special cracking and crushing capabilities. The most important aspect of this element is the treatment of nonlinear material properties. The concrete is capable of cracking (in three orthogonal directions), crushing, plastic deformation, and creep. The rebar are capable of tension and compression, but not shear. They are also capable of plastic deformation and creep. See SOLID65 in the Mechanical APDL Theory Reference for more details about this element.

Figure 65.1:  SOLID65 Geometry

SOLID65 Geometry

SOLID65 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 65.1: SOLID65 Geometry. The element is defined by eight nodes and the isotropic material properties. The element has one solid material and up to three rebar materials. Use the MAT command to input the concrete material properties. Rebar specifications, which are input as real constants, include the material number (MAT), the volume ratio (VR), and the orientation angles (THETA, PHI). The rebar orientations can be graphically verified with the /ESHAPE command.

The volume ratio is defined as the rebar volume divided by the total element volume. The orientation is defined by two angles (in degrees) from the element coordinate system. The element coordinate system orientation is as described in Coordinate Systems. A rebar material number of zero or equal to the element material number removes that rebar capability.

Additional concrete material data, such as the shear transfer coefficients, tensile stresses, and compressive stresses are input in the data table, for convenience, as described in Table 65.1: SOLID65 Concrete Material Data. Typical shear transfer coefficients range from 0.0 to 1.0, with 0.0 representing a smooth crack (complete loss of shear transfer) and 1.0 representing a rough crack (no loss of shear transfer). This specification may be made for both the closed and open crack. When the element is cracked or crushed, a small amount of stiffness is added to the element for numerical stability. The stiffness multiplier CSTIF is used across a cracked face or for a crushed element, and defaults to 1.0E-6.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 65.1: SOLID65 Geometry. 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.

Use the BETAD command to specify the global value of damping. If MP,BETD is defined for the material number of the element (assigned with the MAT command), it is summed with the value from the BETAD command. Similarly, use the TREF command to supply the global value of reference temperature. If MP,REFT is defined for the material number of the element, it is used for the element instead of the value from the TREF command. But if MP,REFT is defined for the material number of the rebar, it is used instead of either the global or element value.

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

The stress relaxation associated with KEYOPT(7) = 1 is used only to help accelerate convergence of the calculations when cracking is imminent. (A multiplier for the amount of tensile stress relaxation can be input as constant C9 in the data table; see Table 65.1: SOLID65 Concrete Material Data) The relaxation does not represent a revised stress-strain relationship for post-cracking behavior. After the solution converges to the cracked state, the modulus normal to the crack face is set to zero. Thus, the stiffness is zero normal to the crack face. See the Mechanical APDL Theory Reference for details.

The program warns when each unreinforced element crushes at all integration points. If this warning is unwanted, it can be suppressed with KEYOPT(8) = 1.

If solution convergence is a problem, set KEYOPT(3) = 2 and apply the load in very small load increments.

Pressure load stiffness effects are included in linear eigenvalue buckling automatically. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

A summary of the element input is given in "SOLID65 Input Summary". A general description of element input is given in Element Input.

SOLID65 Input Summary


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

Degrees of Freedom


Real Constants

(where MATn is material number, VRn is volume ratio, and THETAn and PHIn are orientation angles for up to 3 rebar materials)

Material Properties
TB command: See Element Support for Material Models for this element.
MP command: EX, ALPX (or CTEX or THSX), PRXY or NUXY, DENS (for concrete),
EX, ALPX (or CTEX or THSX), DENS (for each rebar), ALPD
Specify BETD and DMPR only once for the element. (Issue the MAT command to assign the material property set.) REFT may be specified once for the element, or may be assigned on a per-rebar basis. See the discussion in "SOLID65 Input Data" for more information.
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), FL(J), FL(K), FL(L), FL(M), FL(N), FL(O), FL(P)

Special Features
Adaptive descent
Birth and death
Large deflection
Large strain
Stress stiffening

Extra displacement shapes:

0 -- 

Include extra displacement shapes

1 -- 

Suppress extra displacement shapes


Behavior of totally crushed unreinforced elements:

0 -- 


1 -- 

Suppress mass and applied loads, and warning message (see KEYOPT(8))

2 -- 

Features of 1 and apply consistent Newton-Raphson load vector.


Concrete linear solution output:

0 -- 

Print concrete linear solution only at centroid

1 -- 

Repeat solution at each integration point

2 -- 

Nodal stress printout


Concrete nonlinear solution output:

0 -- 

Print concrete nonlinear solution only at centroid

3 -- 

Print solution also at each integration point


Stress relaxation after cracking:

0 -- 

No tensile stress relaxation after cracking

1 -- 

Include tensile stress relaxation after cracking to help convergence


Warning message for totally crushed unreinforced element:

0 -- 

Print the warning

1 -- 

Suppress the warning

SOLID65 Concrete Information

The data listed in Table 65.1: SOLID65 Concrete Material Data is entered in the data table with the TB commands. Data not input are assumed to be zero, except for defaults described below. The constant table is started by using the TBcommand (with Lab = CONCR). Up to eight constants may be defined with the TBDATA commands following a temperature definition on the TBTEMP command. Up to six temperatures (NTEMP = 6 maximum on the TB command) may be defined with the TBTEMP commands. The constants (C1-C9) entered on the TBDATA commands (6 per command), after each TBTEMP command, are:

Table 65.1:  SOLID65 Concrete Material Data

Constant Meaning
1Shear transfer coefficients for an open crack.
2Shear transfer coefficients for a closed crack.
3Uniaxial tensile cracking stress.
4Uniaxial crushing stress (positive).
5Biaxial crushing stress (positive).
6Ambient hydrostatic stress state for use with constants 7 and 8.
7Biaxial crushing stress (positive) under the ambient hydrostatic stress state (constant 6).
8Uniaxial crushing stress (positive) under the ambient hydrostatic stress state (constant 6).
9Stiffness multiplier for cracked tensile condition, used if KEYOPT(7) = 1 (defaults to 0.6).

Absence of the data table removes the cracking and crushing capability. A value of -1 for constant 3 or 4 also removes the cracking or crushing capability, respectively. If constants 1-4 are input and constants 5-8 are omitted, the latter constants default as discussed in the Mechanical APDL Theory Reference. If any one of Constants 5-8 are input, there are no defaults and all 8 constants must be input.

SOLID65 Output Data

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

Several items are illustrated in Figure 65.2: SOLID65 Stress Output. The element stress directions are parallel to the element coordinate system. Nonlinear material printout appears only if nonlinear properties are specified. Rebar printout appears only for the rebar defined. If cracking or crushing is possible, printout for the concrete is also at the integration points, since cracking or crushing may occur at any integration point. The PLCRACK command can be used in POST1 to display the status of the integration points. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 65.2:  SOLID65 Stress Output

SOLID65 Stress Output

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 65.2:  SOLID65 Element Output Definitions

Name Definition O R
ELElement numberYY
NODESNodes - I, J, K, L, M, N, O, PYY
MATMaterial numberYY
NREINFNumber of rebarY-
PRESPressures 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, PYY
TEMPTemperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)YY
FLUENFluences FL(I), FL(J), FL(K), FL(L), FL(M), FL(N), FL(O), FL(P)YY
XC, YC, ZCLocation where results are reportedY 6
S:X, Y, Z, XY, YZ, XZStresses 1 1
S:1, 2, 3Principal stresses 1 1
S:INTStress intensity 1 1
S:EQVEquivalent stress 1 1
EPEL:X, Y, Z, XY, YZ, XZElastic strains 1 1
EPEL:1, 2, 3Principal elastic strains 1 -
EPEL:EQVEquivalent elastic strains [7] 1 1
EPTH:X, Y, Z, XY, YZ, XZAverage thermal strains 1 1
EPTH:EQVEquivalent thermal strains [7] 1 1
EPPL:X, Y, Z, XY, YZ, XZAverage plastic strains 4 4
EPPL:EQVEquivalent plastic strains [7] 4 4
EPCR:X, Y, Z, XY, YZ, XZAverage creep strains 4 4
EPCR:EQVEquivalent creep strains [7] 4 4
NL:EPEQAverage equivalent plastic strain 4 4
NL:SRATRatio of trial stress to stress on yield surface 4 4
NL:SEPLAverage equivalent stress from stress-strain curve 4 4
NL:HPRESHydrostatic pressure- 4
THETCR, PHICRTHETA and PHI angle orientations of the normal to the crack plane 1 1
STATUSElement status 2 2
IRFRebar number 3 -
MATMaterial number 3 -
VRVolume ratio 3 -
THETAAngle of orientation in X-Y plane 3 -
PHIAngle of orientation out of X-Y plane 3 -
EPELUniaxial elastic strain 3 -
SUniaxial stress 3 -
EPELAverage uniaxial elastic strain 5 5
EPPLAverage uniaxial plastic strain 5 5
SEPLAverage equivalent stress from stress-strain curve 5 5
EPCRAverage uniaxial creep strain 5 5

  1. Concrete solution item (output for each integration point (if KEYOPT(5) = 1) and the centroid)

  2. The element status table (Table 65.4: SOLID65 Element Status Table) uses the following terms:

    • Crushed - solid is crushed.

    • Open - solid is cracked and the crack is open.

    • Closed - solid is cracked but the crack is closed.

    • Neither - solid is neither crushed nor cracked.

  3. Rebar solution item repeats for each rebar

  4. Concrete nonlinear integration point solution (if KEYOPT(6) = 3 and the element has a nonlinear material)

  5. Rebar nonlinear integration point solution (if KEYOPT(6) = 3 and the rebar has a nonlinear material)

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

  7. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY); for plastic and creep this value is set at 0.5.

Table 65.3:  SOLID65 Miscellaneous Element Output

Description Names of Items Output O R
Nodal Stress SolutionTEMP, S(X, Y, Z, XY, YZ, XZ), SINT, SEQV 1 -

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

Table 65.4:  SOLID65 Element Status Table

Status Status in Direction 1 Status in Direction 2 Status in Direction 3

Table 65.5: SOLID65 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 65.5: SOLID65 Item and Sequence Numbers:


output quantity as defined in the Table 65.2: SOLID65 Element Output Definitions


predetermined Item label for ETABLE command


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


sequence number for Integration Point solution items

Table 65.5:  SOLID65 Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input
Item Rebar 1 Rebar 2 Rebar 3

Output Quantity Name ETABLE and ESOL Command Input
Item I J K L M N O P
Output Quantity Name ETABLE and ESOL Command Input
Item Integration Point
1 2 3 4 5 6 7 8
Dir 1THETCRNMISC54616875828996103
Dir 2THETCRNMISC56637077849198105
Dir 3THETCRNMISC586572798693100107

SOLID65 Assumptions and Restrictions

  • Zero volume elements are not allowed.

  • Elements may be numbered either as shown in Figure 65.1: SOLID65 Geometry or may have the planes IJKL and MNOP interchanged. Also, the element may not be twisted such that the element has two separate volumes. This occurs most frequently when the elements are not numbered properly.

  • 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 Degenerated Shape Elements). A tetrahedron shape is also available. The extra shapes are automatically deleted for tetrahedron elements.

  • Whenever the rebar capability of the element is used, the rebar are assumed to be "smeared" throughout the element. The sum of the volume ratios for all rebar must not be greater than 1.0.

  • The element is nonlinear and requires an iterative solution.

  • When both cracking and crushing are used together, care must be taken to apply the load slowly to prevent possible fictitious crushing of the concrete before proper load transfer can occur through a closed crack. This usually happens when excessive cracking strains are coupled to the orthogonal uncracked directions through Poisson's effect. Also, at those integration points where crushing has occurred, the output plastic and creep strains are from the previous converged substep. Furthermore, when cracking has occurred, the elastic strain output includes the cracking strain. The lost shear resistance of cracked and/or crushed elements cannot be transferred to the rebar, which have no shear stiffness.

  • The following two options are not recommended if cracking or crushing nonlinearities are present:

    • Stress-stiffening effects.

    • Large strain and large deflection. Results may not converge or may be incorrect, especially if significantly large rotation is involved.

SOLID65 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 Mechanical Premium 

  • Birth and death is not available.

  • Creep is not available.

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