Products: Abaqus/Explicit Abaqus/CAE
You must specify a list of materials that may be present in the Eulerian element. You can also assign a material instance name to each material (see “Eulerian section definition” in “Eulerian analysis,” Section 13.1.1).
| Input File Usage: | *EULERIAN SECTION |
| Abaqus/CAE Usage: | Property module: Create Section: select Solid as the section Category and Eulerian as the section Type |
Distributed loads are available for Eulerian elements. They are specified as described in “Distributed loads,” Section 30.4.3.
Load ID (*DLOAD): BX
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Body force in global X-direction.
Load ID (*DLOAD): BY
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Body force in global Y-direction.
Load ID (*DLOAD): BZ
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Body force in global Z-direction.
Load ID (*DLOAD): BXNU
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Nonuniform body force in global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.
Load ID (*DLOAD): BYNU
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Nonuniform body force in global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.
Load ID (*DLOAD): BZNU
Abaqus/CAE Load/Interaction: Body force
Units: FL–3
Description: Nonuniform body force in global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.
Load ID (*DLOAD): GRAV
Abaqus/CAE Load/Interaction: Gravity
Units: LT–2
Description: Gravity loading in a specified direction (magnitude is input as acceleration).
Load ID (*DLOAD): Pn
Abaqus/CAE Load/Interaction: Pressure
Units: FL–2
Description: Pressure on face n.
Load ID (*DLOAD): PnNU
Abaqus/CAE Load/Interaction: Not supported
Units: FL–2
Description: Nonuniform pressure on face n with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.
Load ID (*DLOAD): SBF
Abaqus/CAE Load/Interaction: Not supported
Units: FL–5T2
Description: Stagnation body force in global X-, Y-, and Z-directions.
Load ID (*DLOAD): SPn
Abaqus/CAE Load/Interaction: Not supported
Units: FL–4T2
Description: Stagnation pressure on face n.
Load ID (*DLOAD): TRSHRn
Abaqus/CAE Load/Interaction: Surface traction
Units: FL–2
Description: Shear traction on face n.
Load ID (*DLOAD): TRVECn
Abaqus/CAE Load/Interaction: Surface traction
Units: FL–2
Description: General traction on face n.
Load ID (*DLOAD): VBF
Abaqus/CAE Load/Interaction: Not supported
Units: FL–4T
Description: Viscous body force in global X-, Y-, and Z-directions.
Load ID (*DLOAD): VPn
Abaqus/CAE Load/Interaction: Not supported
Units: FL–3T
Description: Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion.
Surface-based distributed loads are available for Eulerian elements. They are specified as described in “Distributed loads,” Section 30.4.3.
Load ID (*DSLOAD): P
Abaqus/CAE Load/Interaction: Pressure
Units: FL–2
Description: Pressure on the element surface.
Load ID (*DSLOAD): PNU
Abaqus/CAE Load/Interaction: Pressure
Units: FL–2
Description: Nonuniform pressure on the element surface with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.
Load ID (*DSLOAD): SP
Abaqus/CAE Load/Interaction: Pressure
Units: FL–4T2
Description: Stagnation pressure on the element surface.
Load ID (*DSLOAD): TRSHR
Abaqus/CAE Load/Interaction: Surface traction
Units: FL–2
Description: Shear traction on the element surface.
Load ID (*DSLOAD): TRVEC
Abaqus/CAE Load/Interaction: Surface traction
Units: FL–2
Description: General traction on the element surface.
Load ID (*DSLOAD): VP
Abaqus/CAE Load/Interaction: Pressure
Units: FL–3T
Description: Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion.
A set of output variables is written for each Eulerian material instance listed in the Eulerian section definition. The output variable names are automatically appended with the material instance names. For example, if you define material instances named “steel” and “tin” and request stress output, the first stress components will be written to separate output variables named “S11_steel” and “S11_tin.”
All output is given in global coordinates.
Stress and other tensors (excluding total strain tensors) are available. All tensors have the same components. For example, the stress components are as follows:
S11 |
|
S22 |
|
S33 |
|
S12 |
|
S13 |
|
S23 |
|
Several output variables are also available as element-averaged quantities. These variables are computed as a volume fraction weighted average of all materials present in the element. Use of these variables can substantially decrease the size of the output database for models with many Eulerian materials. For example:
SVAVG | Volume fraction averaged stress. |
, direct stress.
, direct stress.
, direct stress.
, shear stress.
, shear stress.
, shear stress.