SOLID98
## SOLID98 Element Description

## SOLID98 Input Data

### SOLID98 Input Summary

## SOLID98 Output Data

## SOLID98 Assumptions and Restrictions

**Tetrahedral
Coupled-Field Solid**

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

Although this legacy element is available for use in your analysis, ANSYS, Inc. recommends using a current-technology element such as SOLID227. |

SOLID98 is a 10-node tetrahedral version of the 8-node SOLID5 element. The element has a quadratic displacement behavior and is well suited to model irregular meshes (such as produced from various CAD/CAM systems). When used in structural and piezoelectric analyses, SOLID98 has large deflection and stress stiffening capabilities.

The element is defined by ten nodes with up to six degrees of
freedom at each node (see KEYOPT(1)). See SOLID98 in the *Mechanical APDL Theory Reference* for more
details about this element. The 3-D magnetic, thermal, electric,
piezoelectric, and structural field capability is similar to that
described for SOLID5.

The geometry, node locations, and the coordinate system for this element are shown in Figure 98.1: SOLID98 Geometry. The element input data is essentially the same as for SOLID5 except that there are 10 nodes instead of 8.

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). Nonlinear magnetic B-H, 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 can be specified per material.

Element loads are described in Nodal 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 98.1: SOLID98 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 temperatures 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 loading.

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.

A summary of the element input is given in "SOLID98 Input Summary". A general description of element input is given in Element Input.

**Nodes**I, J, K, L, M, N, O, P, Q, R

**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, NTH, MUZERO, MURX, MURY, MURZ, RSVX, RSVY, RSVZ, E, MGXX, MGYY, MGZZ, PERX, PERY, PERZ, DMPR**Surface Loads****Pressure, Convection or Heat Flux (but not both), Radiation (using Lab = RDSF), and Maxwell Force Flags --**face 1 (J-I-K), face 2 (I-J-L), face 3 (J-K-L), face 4 (K-I-L)

**Body Loads****Temperatures --**T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P), T(Q), T(R)

**Heat Generations --**HG(I), HG(J), HG(K), HG(L), HG(M), HG(N), HG(O), HG(P), HG(Q), HG(R)

**MVDI --**VD(I), VD(J), VD(K), VD(L), VD(M), VD(N), VD(O), VD(P), VD(Q), VD(R)

**EF --**EFX, EFY, EFZ. See "SOLID98 Assumptions and Restrictions".

**Special Features**Adaptive descent Birth and death Large deflection Stress stiffening **KEYOPT(1)**Degree of freedom selection:

**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)**Specific heat matrix:

**0 --**Consistent specific heat matrix

**1 --**Diagonalized specific heat matrix

**KEYOPT(5)**Extra element output:

**0 --**Basic element printout

**2 --**Nodal stress or magnetic field printout

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 98.1: SOLID98 Element Output Definitions

Several items are illustrated in Figure 98.2: SOLID98 Element Output. The component output 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 number refers to a table footnote
that describes when the item is *conditionally* available, and “-” indicates that the item is *not* available.

**Table 98.1: SOLID98 Element Output Definitions**

Name | Definition | O | R |
---|---|---|---|

EL | Element Number | Y | Y |

NODES | Corner nodes - I, J, K, L | Y | Y |

MAT | Material number | Y | Y |

VOLU: | Volume | Y | Y |

XC, YC, ZC | Location where results are reported | Y | 3 |

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

TEMP(INPUT) | Temperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P), T(Q), T(R) | Y | Y |

HGEN(INPUT) | Heat generations HG(I), HG(J), HG(K), HG(L), HG(M), HG(N), HG(O), HG(P), HG(Q), HG(R) | Y | - |

S:X, Y, Z, XY, YZ, XZ | 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 strain [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 |

Combined (FJB or FMX) force components | Combined (FJB or FMX) force components | - | 1 |

EF:X, Y, Z | Electric field components | 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 |

U(E, D, M) | 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 |

Table 98.3: SOLID98 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 98.3: SOLID98 Item and Sequence Numbers:

**Name**output quantity as defined in Table 98.1: SOLID98 Element Output Definitions

**Item**predetermined Item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

**I,J,...,L**sequence number for data at nodes I,J,...,L

**FC***n*-sequence number for solution items for element Face

*n*

The element requires an iterative solution for field coupling (displacement, temperature, electric, magnetic, but not piezoelectric)

When using SOLID98 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. Elements may be numbered either as shown in Figure 98.1: SOLID98 Geometry or may have node L below the IJK plane.

An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. See Quadratic Elements (Midside Nodes) for more information about the use of midside nodes.

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.

Temperatures and heat generation rates, if internally calculated, include any user defined heat generation rates.

Large-deflection capabilities available for KEYOPT(1) = 2 and 3 are not available for KEYOPT(1) = 0. Stress stiffening is available for KEYOPT(1) = 0, 2, and 3.

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.