/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  
I_{solid}  I_{smstr}  I_{cstr}  I_{npts}  I_{int}  d_{n}  
q_{a}  q_{b}  h  
$\text{\Delta}{t}_{\mathrm{min}}$ 
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) 

I_{solid}  Solid elements formulation flag.
(Integer) 

I_{smstr}  Strain formulation flag.
4
(Integer) 

I_{cstr}  Constant stress
formulation flag to indicate the thickness direction. Only valid for
I_{solid} =14. 2
(Integer) 

I_{npts}  Number of integration
points.
(Integer) Where:


I_{int}  Thickness integration
formulation. Only valid for I_{solid} =16.
(Integer) 

d_{n}  Numerical damping for
stabilization. Only valid for I_{solid} =15. Default = 0.1 (Real) 

q_{a}  Quadratic bulk
viscosity. Default = 1.10 (Real) Default = 0.0 for /MAT/LAW70 (FOAM_TAB) 

q_{b}  Linear bulk
viscosity. Default = 0.05 (Real) Default = 0.0 for /MAT/LAW70 

h  Hourglass viscosity
coefficient. Default = 0.10 (Real) 

$\text{\Delta}{t}_{\mathrm{min}}$  Minimum time
step Default = 10^{6} (Real) 
$\left[\text{s}\right]$ 
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 I_{solid}=14 (HA8), a
different thickness direction can be specified using the constant stress
flag, I_{cstr}. Note: Check the elements local system orientation using a preprocessor.
 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)
 I_{cstr}  for reduced stress
integration.For I_{solid}=14 (HA8) the reduced integration direction and thus thickness direction of the shell can be set by parameter I_{cstr}. This parameter represents a 3digit sequence of "0" and "1", which corresponds to standard rst 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 I_{smstr} = I_{cpre} = I_{frame}=1, the values for these options are defined using the best options based on the element formulation, element type, and material. Alternatively, defining I_{smstr} = I_{cpre} = I_{frame}=2 will overwrite the values for these options defined in this property with the best value (/DEF_SOLID) 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.
 I_{solid}  Solid elements
formulation flag.
 For I_{solid}=15, parameter I_{cstr} 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 I_{solid} =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 I_{solid}=15 with pentahedron elements, /PENTA6 elements are recommended but degenerated /BRICK elements can also be used.
 I_{smstr}
 Small strain formulation flag.
 If the small strain option is set (I_{smstr} =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 I_{solid} =14 (HA8) and I_{solid} =15 (HSEPH).
 The Radioss Engine option /DT/BRICK/CST will only work for brick property sets with I_{smstr} =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 I_{solid} =14, 15 Full geometric nonlinearities I_{smstr} = 2, 4
Switch to small strain using element shape from cycle before negative volume.
 Numerical damping d_{n} is only used in hourglass stress calculation for HSEPH (I_{solid} =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
postprocessing.
 For postprocessing solid element stress, refer to /ANIM/BRICK/TENS/STRESS and /H3D/SOLID/TENS/STRESS for animation and /TH/BRICK for plot files.