/PROP/TYPE20 (TSHELL)
Block Format Keyword This property is used to define the general thick shell property set.
Format
(1) | (2) | (3) | (4) | (5) | (6) | (7) | (8) | (9) | (10) |
---|---|---|---|---|---|---|---|---|---|
/PROP/TYPE20/prop_ID/unit_ID or /PROP/TSHELL/prop_ID/unit_ID | |||||||||
prop_title | |||||||||
Isolid | Ismstr | Icstr | Inpts | Iint | dn | ||||
qa | qb | h | |||||||
Definitions
Field | Contents | SI Unit Example |
---|---|---|
prop_ID | Property
identifier. (Integer, maximum 10 digits) |
|
unit_ID | Unit Identifier. (Integer, maximum 10 digits) |
|
prop_title | Property
title. (Character, maximum 100 characters) |
|
Isolid | Solid elements formulation flag.
(Integer) |
|
Ismstr | Strain formulation flag.
4
(Integer) |
|
Icstr | Constant stress
formulation flag to indicate the thickness direction. Only valid for
Isolid =14. 2
(Integer) |
|
Inpts | Number of integration
points.
(Integer) Where:
|
|
Iint | Thickness integration
formulation. Only valid for Isolid =16.
(Integer) |
|
dn | Numerical damping for
stabilization. Only valid for Isolid =15. Default = 0.1 (Real) |
|
qa | Quadratic bulk
viscosity. Default = 1.10 (Real) Default = 0.0 for /MAT/LAW70 (FOAM_TAB) |
|
qb | Linear bulk
viscosity. Default = 0.05 (Real) Default = 0.0 for /MAT/LAW70 |
|
h | Hourglass viscosity
coefficient. Default = 0.10 (Real) |
|
Minimum time
step Default = 106 (Real) |
Comments
- Thickness direction:
- By default, the element must be oriented so that the thickness direction of the thick shell is in the elements "s" direction.
- However, when using Isolid=14 (HA8), a
different thickness direction can be specified using the constant stress
flag, Icstr. Note: Check the elements local system orientation using a pre-processor.
- r, s, t
- Isoparametric frame
- r
- Center of (1, 2, 6, 5) to center of (4, 3, 7, 8)
- s
- Center of (1, 2, 3, 4) to center of (5, 6, 7, 8)
- t
- Center of (1, 4, 8, 5) to center of (2, 3, 7, 6)
- Icstr - for reduced stress
integration.For Isolid=14 (HA8) the reduced integration direction and thus thickness direction of the shell can be set by parameter Icstr. This parameter represents a 3-digit sequence of "0" and "1", which corresponds to standard r-s-t elemental coordinate system for solid elements.
- 0
- No reduced stress integration is done in corresponding direction.
- 1
- Reduced integration is used in this direction.
For example:
"010" means that reduced integration is used, and the thickness direction corresponds to element axis "s".
- When using the automatic setting option Ismstr = Icpre = Iframe=-1, the values for these options are defined using the best options based on the element formulation, element type, and material. Alternatively, defining Ismstr = Icpre = Iframe=-2 will overwrite the values for these options defined in this property with the best value based on element type and material law. To see the values defined by Radioss, review the “PART ELEMENT/MATERIAL PARAMETER REVIEW” section of the Starter output file.
- Isolid - Solid elements
formulation flag.
- For Isolid=15, parameter Icstr has no effect. It is always assumed that elemental direction "s" uses reduced integration and is the thickness direction.
- When property is used with /MAT/LAW1 (ELAST), with Isolid =15 and number of integration points is different from one, number of integration points is set to 2 (enough to compute correct bending).
- When using Isolid=15 with pentahedron elements, /PENTA6 elements are recommended but degenerated /BRICK elements can also be used.
- Ismstr
- Small strain formulation flag.
- If the small strain option is set (Ismstr =1, 3), the strains and stresses used in material laws are engineering strains and stresses. Otherwise, they are true strains and stresses.
- The small strain option is available for Isolid =14 (HA8) and Isolid =15 (HSEPH).
- The Radioss Engine option /DT/BRICK/CST will only work for brick property sets with Ismstr =2
- Starting with version 2017, Lagrangian elements whose volume becomes
negative during a simulation will automatically switch strain
formulations to allow the simulation to continue. When this occurs, a
WARNING message will be printed in the Engine output file. The following
options are supported.
Element Type Element Formulation Strain Formulation Negative Volume Handling Method /BRICK Isolid =14, 15 Full geometric nonlinearities Ismstr = 2, 4
Switch to small strain using element shape from cycle before negative volume.
- Numerical damping dn is only used in hourglass stress calculation for HSEPH (Isolid =15).
- Hourglass viscosity coefficient h must have a value between 0 and 0.15 and is not active with 8 integration point solids.
- Output for
post-processing.
- For post-processing solid element stress, refer to /ANIM/BRICK/TENS/STRESS and /H3D/SOLID/TENS/STRESS for animation and /TH/BRICK for plot files.