/PROP/TYPE21 (TSH_ORTH)
Block Format Keyword This property is used to define the orthotropic thick shell property set.
Format
(1)  (2)  (3)  (4)  (5)  (6)  (7)  (8)  (9)  (10) 

/PROP/TYPE21/prop_ID/unit_ID or /PROP/TSH_ORTH/prop_ID/unit_ID  
prop_title  
I_{solid}  I_{smstr}  I_{cstr}  I_{npts}  d_{n}  
q_{a}  q_{b}  
V_{X}  V_{Y}  V_{Z}  Skew_ID  I_{orth}  
$\varphi $  
$\text{\Delta}{t}_{\mathrm{min}}$ 
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}  Small strain formulation
flag. 3
(Integer) 

I_{cstr}  Constant stress
formulation flag. Only valid for I_{solid} = 14 (HA8 only). 1
(Integer) 

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


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 

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

V_{X}  X component for reference
vector. (Real) 

V_{Y}  Y component for reference
vector. (Real) 

V_{Z}  Z component for reference
vector. (Real) 

Skew_ID  Skew identifier. If the local skew has been defined, its Xaxis replaces the reference vector (V_{X}, V_{Y}, and V_{Z} will be ignored). (Integer) 

I_{orth}  Orthotropic system
formulation flag for reference vector.
(Integer) 

$\varphi $  Angle of the first
direction of orthotropy. (Real) 
$\left[\mathrm{deg}\right]$ 
$\text{\Delta}{t}_{\mathrm{min}}$  Minimum time
step. Default = 10^{6} (Real) 
$\left[\text{s}\right]$ 
Example
#RADIOSS STARTER
#12345678910
# 1. SKEWS & FRAMES:
#12345678910
/SKEW/FIX/1
New SKEW 1
# OX OY OZ
0 100 0
# X1 Y1 Z1
1 1 0
# X2 Y2 Z2
.408248290463863 .408248290463863 .816496580927726
#12345678910
# 2. LOCAL_UNIT_SYSTEM:
#12345678910
/UNIT/2
unit for prop
# MUNIT LUNIT TUNIT
kg mm ms
#12345678910
# 3. GEOMETRICAL SETS:
#12345678910
/PROP/TYPE21/1/2
TSH_ORTH example
# Isolid Ismstr Icstr Inpts dn
14 0 010 222 0
# q_a q_b
0 0
# Vx Vy Vz skew_ID Iorth
0 0 0 1 0
# Ortho_angle
90
# dt_min
0
#12345678910
#enddata
#12345678910
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_{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.
 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.
 I_{solid}  Solid elements formulation flag.
 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.
 Othotropy in local coordinate
system.
 The thick shell orthotropy is planar and the third orthotropy direction is coincident with the normal to the shell plane.
 Global vector $V$ or skew_ID is used to define the othotropy direction.
 $\varphi $
is the angle between the first direction of
orthotropy and projection of reference vector on the shell mean plane (r
and t). It is given in degrees.
 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.