/PROP/TYPE21 (TSH_ORTH)

Format

Definitions

Example

Figure 1. Skew and Angle $\varphi$ to Define the Material Direction (Fiber Direction) m1

#RADIOSS STARTER
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
#-  1. SKEWS & FRAMES:
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
/SKEW/FIX/1
New SKEW 1
#                 OX                  OY                  OZ
                   0                 100                   0
#                 X1                  Y1                  Z1
                   1                   1                   0
#                 X2                  Y2                  Z2
   -.408248290463863    .408248290463863    .816496580927726
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
#-  2. LOCAL_UNIT_SYSTEM:
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
/UNIT/2
unit for prop
#              MUNIT               LUNIT               TUNIT
                  kg                  mm                  ms
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
#-  3. GEOMETRICAL SETS:
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
/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
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|
#enddata
#---1----|----2----|----3----|----4----|----5----|----6----|----7----|----8----|----9----|---10----|

Comments

1. 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 pre-processor.

     
     
     Figure 2.

     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)

2. 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 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".

3. 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 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.
4. 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	Isolid =14, 15	Full geometric nonlinearities Ismstr = 2, 4	Switch to small strain using element shape from cycle before negative volume.

5. 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.
6. 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.

     
     
     Figure 3.

7. 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.