2.14.6. User Defined Results for Explicit Dynamics Analyses

For general information about User Defined Results, see User Defined Results in the ANSYS Mechanical User's Guide

Shown here are the User Defined Results that are specific to an Explicit Dynamics analysis. These User Defined results are not available for analyses using Workbench LS-DYNA.

VariableDescriptionType
BEAM_LEN Beam lengthElement Nodal
BOND_STATUSThe number of nodes bonded to the faces on an element during the analysis. A value of -1 is shown where all the bonds for the face have broken.Elemental
C_S_AREABeam cross section area.Element Nodal
COMPRESS

Material compression:

Compression, μ = ρ/ρ0 .

Element Nodal
CROSS_SECTIONBeam cross section number.Elemental
DAMAGE

Material Damage:

0– intact material.

1- fully fractured.

Element Nodal
DENSITYMaterial Density.Element Nodal
EFF_STNEffective Geometric Strain of a cell.Element Nodal
EFF_PL_STNEffective Plastic Strain. Note: This is calculated incrementally, unlike the equivalent plastic strain (EPPLEQV), which is calculated as an instantaneous value.Element Nodal
ENERGY_DAMEnergy resulting from fracture for the Johnson-Holmquist brittle strength model.Element Nodal
EROSION

Erosion Status:

0 - no erosion.

>0 - eroded (will not be displayed).

Elemental
EPS_RATEEffective Plastic Strain Rate.Element Nodal
F_AXIALBeam axial force.Element Nodal
INT_ENERGYInternal energy of the material.Element Nodal
MASSMass of material in an element.Element Nodal
MATERIAL

Material index. The material index as defined in the Explicit solver. There is not always a direct one-to-one correlation with materials defined in Engineering Data and those used in the Explicit solver.

For layered section shells, the MATERIAL for individual layers can be shown by using the Layer property in the results details view.

Elemental
MOM_TORBeam rotation inertia.Element Nodal
POROSITY

Material Porosity:

Porosity, α = ρSolid/ρ

Elemental
PRESSUREPressure.Element Nodal
PRES_BULKDilation pressure for the Johnson-Holmquist brittle strength model.Elemental
SOUNDSPEEDMaterial soundspeed.Element Nodal
STATUS

Material Status:

1 – elastic.

2 – undergoing plastic flow.

3 – failed due to effective criteria (with healing).

4 – failed due to effective criteria.

5 – failed due to stress/strain in principal direction 1.

6 – failed due to stress/strain in principal direction 2.

7 – failed due to stress/strain in principal direction 3.

8 – failed due to shear stress/strain in principal direction 12.

9 – failed due to shear stress/strain in principal direction 23.

10 – failed due to shear stress/strain in principal direction 31.

For layered section shells, the STATUS for individual layers can be shown by selecting the Layer number in the results details view.

Elemental
STOCH_FACTStochastic factor applied when the stochastic property as defined in the material failure model.Elemental
STRAIN_XXTotal strain XX.Element Nodal
STRAIN_YYTotal strain YY.Element Nodal
STRAIN_ZZTotal strain ZZ.Element Nodal
STRAIN_XYTotal strain XY. These are tensor shear strains, and not engineering shear strains.Element Nodal
STRAIN_YZTotal strain YZ. These are tensor shear strains, and not engineering shear strains.Element Nodal
STRAIN_ZXTotal strain ZX. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_X_SHELL_LAYER__#Shell total strain XX, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_Y_SHELL_LAYER__#Shell total strain YY, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_Z_SHELL_LAYER__#Shell total strain ZZ, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_XY_SHELL_LAYER__#Shell total strain XY, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_YZ_SHELL_LAYER__#Shell total strain YZ, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUB_STN_ZX_SHELL_LAYER__#Shell total strain ZX, sub-layer #. These are tensor shear strains, and not engineering shear strains.Element Nodal
SUBL_EPS_SHELL_LAYER_#Effective plastic strain, sub-layer number.Element Nodal
TEMPERATUREMaterial Temperature.Element Nodal
THICKNESSShell Thickness.Element Nodal
TYPE

Element category (element number returned):

HEX: 100-101.

PENTA: 102.

TET: 103-104,106.

PYRAMID: 105.

QUAD: 107.

TRI: 108.

SHL: 200-202, 204.

BEAM: 203.

Elemental
VISC_PRESViscous pressure due to artificial viscosity. No results will display for an Eulerian part.Element Nodal
VTXXViscoelastic stress XX.Element Nodal
VTYYViscoelastic stress YY.Element Nodal
VTZZViscoelastic stress ZZ.Element Nodal
VTXYViscoelastic stress XY.Element Nodal
VTYZViscoelastic stress YZ.Element Nodal
VTZXViscoelastic stress ZX.Element Nodal

For Euler (Virtual) Analyses

The following results are multi-material variables:

For each Eulerian (Virtual) body in the analysis, a separate component will be available, which will allow the user to plot the result for the particular material associated with that body. The component name will be derived from the body name. There will also be an “ALL” component, which will displays results for all materials. Results for Lagrangian bodies can be viewed by selecting this “ALL” component. For a purely Lagrangian analysis, only the “ALL” component will be available to the user.

For example, an analysis has two Eulerian (Virtual) bodies (Solid, Solid) and a Lagrangian Body (Surface Body), as shown in the image of the Outline View below.

In the User Defined Result Expression Worksheet, there are three components available for the multi-material results named SOLID, SOLID_2, and ALL.


Note:  It may be necessary to delete and reinsert multi-material results in order to view result for databases created prior to Release 13.0


For NBS Tetrahedral Elements

The element variables listed below can be used to visualize the variable values at the nodes. The variable values presented in the element are a volume weighted average of those at the nodes.

The following variables are available as calculated directly from the solver in the element:


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