SOLID5
3D Coupled-Field Solid
SOLID5 Element Description
| Although this element is available for use in your analysis, Ansys, Inc. recommends using a current-technology element such as SOLID226. |
SOLID5 has a 3D magnetic, thermal, electric, piezoelectric, and structural field capability with limited coupling between the fields. The element has eight nodes with up to six degrees of freedom at each node. Scalar potential formulations (reduced RSP, difference DSP, or general GSP) are available for modeling magnetostatic fields in a static analysis. When used in structural and piezoelectric analyses, SOLID5 has large deflection and stress stiffening capabilities. See SOLID5 in the Mechanical APDL Theory Reference for more details about this element. Coupled field elements with similar field capabilities are PLANE13, and SOLID98.
SOLID5 Input Data
The geometry, node locations, and the coordinate system for this element are shown in Figure 5.1: SOLID5 Geometry. The element is defined by eight nodes and the material properties. The type of units (MKS or user defined) is specified through the EMUNIT command. EMUNIT also determines the value of MUZERO. The EMUNIT defaults are MKS units and MUZERO = 4 π x 10-7 Henries/meter. In addition to MUZERO, orthotropic relative permeability is specified through the MURX, MURY, and MURZ material property labels.
MGXX, MGYY, and MGZZ represent vector components of the coercive force for permanent magnet materials. The magnitude of the coercive force is the square root of the sum of the squares of the components. The direction of polarization is determined by the components MGXX, MGYY, and MGZZ. Permanent magnet polarization directions correspond to the element coordinate directions. Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Coordinate Systems. Nonlinear magnetic, piezoelectric, and anisotropic elastic properties are entered via the TB command. Nonlinear orthotropic magnetic properties can be specified with a combination of a B-H curve and linear relative permeability. The B-H curve is used in each element coordinate direction where a zero value of relative permeability is specified. Only one B-H curve may be specified per material.
Various combinations of nodal loading are available for this
element (depending upon the KEYOPT(1) value). Nodal loads are defined
with the D and the F commands.
With the D command, the Lab variable corresponds to the degree of freedom (UX, UY, UZ, TEMP,
VOLT, MAG) and VALUE corresponds to the
value (displacements, temperature, voltage, scalar magnetic potential).
With the F command, the Lab variable corresponds to the force (FX, FY, FZ, HEAT, AMPS, FLUX)
and VALUE corresponds to the value (force,
heat flow, current or charge, magnetic flux).
Element loads are described in Element Loading. Pressure, convection or heat flux (but not both), radiation, and Maxwell force flags may be input on the element faces indicated by the circled numbers in Figure 5.1: SOLID5 Geometry using the SF and SFE commands. Positive pressures act into the element. Surfaces at which magnetic forces are to be calculated may be identified by using the MXWF label on the surface load commands (no value is required.) A maxwell stress tensor calculation is performed at these surfaces to obtain the magnetic forces. These forces are applied in solution as structural loads. The surface flag should be applied to "air" elements adjacent to the body for which forces are required. Deleting the MXWF specification removes the flag.
The body loads, temperature, heat generation rate and magnetic virtual displacement may be input based on their value at the element's nodes or as a single element value (BF and BFE). When the temperature degree of freedom is active (KEYOPT(1) = 0,1 or 8), applied body force temperatures (BF, BFE) are ignored. In general, unspecified nodal values of temperature and heat generation rate default to the uniform value specified with the BFUNIF or TUNIF commands. Calculated Joule heating (JHEAT) is applied in subsequent iterations as heat generation rate.
If the temperature degree of freedom is present, the calculated temperatures override any input nodal temperatures.
Air elements in which Local Jacobian forces are to be calculated may be identified by using nodal values of 1 and 0 for the MVDI label (BF). See the Low-Frequency Electromagnetic Analysis Guide for details. These forces are not applied in solution as structural loads.
Current for the scalar magnetic potential options is defined with the SOURC36 element the command macro RACE, or through electromagnetic coupling. The various types of scalar magnetic potential solution options are defined with the MAGOPT command.
A summary of the element input is given in "SOLID5 Input Summary". A general description of element input is given in Element Input.
SOLID5 Input Summary
- Nodes
I, J, K, L, M, N, O, P
- Degrees of Freedom
UX, UY, UZ, TEMP, VOLT, MAG if KEYOPT (1) = 0 TEMP, VOLT, MAG if KEYOPT (1) = 1 UX, UY, UZ if KEYOPT (1) = 2 UX, UY, UZ, VOLT if KEYOPT(1) = 3 TEMP if KEYOPT (1) = 8 VOLT if KEYOPT (1) = 9 MAG if KEYOPT (1) = 10 - Real Constants
None
- Material Properties
TB command: See Element Support for Material Models for this element. MP command: EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, GXY, GYZ, GXZ, ALPD, BETD, KXX, KYY, KZZ, C, DMPR, DMPS ENTH, MUZERO, MURX, MURY, MURZ, RSVX, RSVY, RSVZ, MGXX, MGYY, MGZZ, PERX, PERY, PERZ) - Surface Loads
- Pressure, Convection or Heat Flux (but not both), Radiation (using Lab = RDSF, see View Factor Updating at the Substep Level for a Coupled-Field Analysis Including Large-deflection Effects in the Thermal Analysis Guide), and Maxwell Force Flags --
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)
- Heat Generations --
HG(I), HG(J), HG(K), HG(L), HG(M), HG(N), HG(O), HG(P)
- Magnetic Virtual Displacements --
VD(I), VD(J), VD(K), VD(L), VD(M), VD(N), VD(O), VD(P)
- Electric Field --
EFX, EFY, EFZ. See "SOLID5 Assumptions and Restrictions".
- Special Features
- KEYOPT(1)
Element degrees of freedom:
- 0 --
UX, UY, UZ, TEMP, VOLT, MAG
- 1 --
TEMP, VOLT, MAG
- 2 --
UX, UY, UZ
- 3 --
UX, UY, UZ, VOLT
- 8 --
TEMP
- 9 --
VOLT
- 10 --
MAG
- KEYOPT(3)
Extra shapes:
- 0 --
Include extra shapes
- 1 --
Do not include extra shapes
- KEYOPT(5)
Extra element output:
- 0 --
Basic element printout
- 2 --
Nodal stress or magnetic field printout
SOLID5 Output Data
The solution output associated with the element is in two forms
Nodal degree of freedom results included in the overall nodal solution
Additional element output as shown in Table 5.1: SOLID5 Element Output Definitions.
Several items are illustrated in Figure 5.2: SOLID5 Element Output. The element stress directions are parallel to the element coordinate system. The reaction forces, heat flow, current, and magnetic flux at the nodes can be printed with the OUTPR command. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.
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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.
Table 5.1: SOLID5 Element Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element Number | Y | Y |
| NODES | Element nodes - I, J, K, L, M, N, O, P | Y | Y |
| MAT | Element material number | Y | Y |
| VOLU: | Element volume | Y | Y |
| XC, YC, ZC | Location where results are reported | Y | 3 |
| PRES | 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 | Input Temperatures: T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P) | Y | Y |
| HGEN | Input Heat Generations: HG(I), HG(J), HG(K), HG(L), HG(M), HG(N), HG(O), HG(P) | Y | Y |
| S:X, Y, Z, XY, YZ, XZ | Component stresses | 1 | 1 |
| S:1, 2, 3 | Principal stresses | 1 | 1 |
| S:INT | Stress intensity | 1 | 1 |
| S:EQV | Equivalent stress | 1 | 1 |
| EPEL:X, Y, Z, XY, YZ, XZ | Elastic strains | 1 | 1 |
| EPEL:1, 2, 3 | Principal elastic strains | 1 | - |
| EPEL:EQV | Equivalent elastic strains [4] | 1 | 1 |
| EPTH:X, Y, Z, XY, YZ, XZ | Thermal strains | 1 | 1 |
| EPTH:EQV | Equivalent thermal strains [4] | 1 | 1 |
| LOC | Output location (X, Y, Z) | 1 | 1 |
| MUX, MUY, MUZ | Magnetic permeability | 1 | 1 |
| H: X, Y, Z | Magnetic field intensity components | 1 | 1 |
| H:SUM | Vector magnitude of H | 1 | 1 |
| B:X, Y, Z | Magnetic flux density components | 1 | 1 |
| B:SUM | Vector magnitude of B | 1 | 1 |
| FJB | Lorentz magnetic force components (X, Y, Z) | 1 | - |
| FMX | Maxwell magnetic force components (X, Y, Z) | 1 | - |
| FVW | Virtual work force components (X, Y, Z) | 1 | 1 |
| FMAG:X, Y, Z | Combined (FJB or FMX) force components | - | 1 |
| EF:X, Y, Z | Electric field components (X, Y, Z) | 1 | 1 |
| EF:SUM | Vector magnitude of EF | 1 | 1 |
| JS:X, Y, Z | Source current density components | 1 | 1 |
| JSSUM | Vector magnitude of JS | 1 | 1 |
| JHEAT: | Joule heat generation per unit volume | 1 | 1 |
| D:X, Y, Z | Electric flux density components | 1 | 1 |
| D:SUM | Vector magnitude of D | 1 | 1 |
| UE, UD, UM | Elastic (UE), dielectric (UD), and electromechanical coupled (UM) energies | 1 | 1 |
| TG:X, Y, Z | Thermal gradient components | 1 | 1 |
| TG:SUM | Vector magnitude of TG | 1 | 1 |
| TF:X, Y, Z | Thermal flux components | 1 | 1 |
| TF:SUM | Vector magnitude of TF (heat flow rate/unit cross-section area) | 1 | 1 |
| FACE | Face label | 2 | 2 |
| AREA | Face area | 2 | 2 |
| NODES | Face nodes | 2 | - |
| HFILM | Film coefficient at each node of face | 2 | - |
| TBULK | Bulk temperature at each node of face | 2 | - |
| TAVG | Average face temperature | 2 | 2 |
| HEAT RATE | Heat flow rate across face by convection | 2 | 2 |
| HEAT RATE/AREA | Heat flow rate per unit area across face by convection | 2 | - |
| HFLUX | Heat flux at each node of face | 2 | - |
| HFAVG | Average film coefficient of the face | 2 | 2 |
| TBAVG | Average face bulk temperature | - | 2 |
| HFLXAVG | Heat flow rate per unit area across face caused by input heat flux | - | 2 |
Element solution at the centroid printed out only if calculated (based on input data).
Nodal stress or magnetic field solution (only if KEYOPT(5) = 2). The solution results are repeated at each node and only if a surface load is input.
Available only at centroid as a *GET item.
The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY).
Table 5.2: SOLID5 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. The following notation is used in Table 5.2: SOLID5 Item and Sequence Numbers:
- Name
output quantity as defined in the Table 5.1: SOLID5 Element Output Definitions
- Item
predetermined Item label for ETABLE command
- E
sequence number for single-valued or constant element data
- I,J,...,P
sequence number for data at nodes I,J,...,P
- FCn
sequence number for solution items for element Face n
Table 5.2: SOLID5 Item and Sequence Numbers
| Output Quantity Name | ETABLE and ESOL Command Input | |||||||||
|---|---|---|---|---|---|---|---|---|---|---|
| Item | E | 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 |
| MUX | NMISC | 1 | - | - | - | - | - | - | - | - |
| MUY | NMISC | 2 | - | - | - | - | - | - | - | - |
| MUZ | NMISC | 3 | - | - | - | - | - | - | - | - |
| FVWX | NMISC | 4 | - | - | - | - | - | - | - | - |
| FVWY | NMISC | 5 | - | - | - | - | - | - | - | - |
| FVWZ | NMISC | 6 | - | - | - | - | - | - | - | - |
| FVWSUM | NMISC | 7 | - | - | - | - | - | - | - | - |
| UE | NMISC | 16 | - | - | - | - | - | - | - | - |
| UD | NMISC | 17 | - | - | - | - | - | - | - | - |
| UM | NMISC | 18 | - | - | - | - | - | - | - | - |
SOLID5 Assumptions and Restrictions
The element requires an iterative solution for field coupling (displacement, temperature, electric, magnetic, but not piezoelectric)
When using SOLID5 with SOURC36 elements, the source elements must be placed so that the resulting Hs field fulfills boundary conditions for the total field.
The element must not have a zero volume or a zero length side. This occurs most frequently when the element is not numbered properly.
Elements may be numbered either as shown in Figure 5.1: SOLID5 Geometry or may have the planes IJKL and MNOP interchanged.
A prism shaped element may be formed by defining duplicate node numbers as described in Degenerated Shape Elements.
The difference scalar magnetic potential option is restricted to singly-connected permeable regions, so that as μ →
in these regions, the resulting field H → 0.
The reduced scalar and general scalar potential options do not have
this restriction.At a free surface of the element (that is, not adjacent to another element and not subjected to a boundary constraint), the normal component of magnetic flux density (B) is assumed to be zero.
Temperatures and heat generation rates, if internally calculated, include any user defined heat generation rates.
The thermal, electrical, magnetic, and structural terms are coupled through an iterative procedure.
Large deflection capabilities available for KEYOPT(1) = 2 and 3 are not available for KEYOPT(1) = 0.
Do not constrain all VOLT DOFs to the same value in a piezoelectric analysis (KEYOPT(1) = 0 or 3). Perform a pure structural analysis instead (KEYOPT(1) = 2).
This element may not be compatible with other elements with the VOLT degree of freedom. To be compatible, the elements must have the same reaction solution for the VOLT DOF. Elements that have an electric charge reaction solution must all have the same electric charge reaction sign. For more information, see Element Compatibility in the Low-Frequency Electromagnetic Analysis Guide.
The electric field body load is not used during solution and is applicable only to POST1 charged particle tracing.
In an MSP analysis, avoid using a closed domain and use an open domain, closed with natural flux parallel boundary conditions on the MAG degree of freedom, or infinite elements. If you use a closed domain, you may see incorrect results when the formulation is applied using SOLID5, SOLID96, or SOLID98 elements and the boundary conditions are not satisfied by the Hs field load calculated by the Biot-Savart procedure based on SOURC36 current source primitive input.
When KEYOPT(1) = 1, 8, 9, or 10:
Stress stiffening is not available.
Birth and death is not available.
KEYOPT(3) is not applicable.