/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        
Δ t min MathType@MTEF@5@5@+= feaagKart1ev2aqatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbbG8FasPYRqj0=yi0dXdbba9pGe9xq=JbbG8A8frFve9 Fve9Ff0dmeaabaqaciGacaGaaeqabaWaaeaaeaaakeaacaqGuoGaam iDamaaBaaaleaaciGGTbGaaiyAaiaac6gaaeqaaaaa@3B70@                

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.
= 0
Use value /DEF/SOLID.
= 14
HA8, 8-node thick shell element, full integration, variable number of Gauss integration points, co-rotational system formulation, shear locking-free.
= 15
HSEPH/PA6 thick shell elements (8-node and 6-node respectively). Co-rotational system formulation, under integrated (1 Gauss point in the plane) with physical hourglass stabilization. Variable number of integration points in thickness direction.
= 16
Quadratic 16-node thick shell, full integration, variable number of Gauss points in all directions.

(Integer)

  
Ismstr Strain formulation flag. 4
= -1
Automatically define the best value based on element type and material law.
= 0
Use value in /DEF_SOLID.
= 1
Small strain from time =0.
= 2
Full geometric nonlinearities with possible small strain formulation in Radioss Engine (/DT/Eltyp/Keyword3/Iflag).
= 3
Simplified small strain formulation from time =0 (non-objective formulation).
= 4 Default, if /DEF_SOLID is not defined
Full geometric nonlinearities (/DT/BRICK/CST has no effect).

(Integer)

  
Icstr Constant stress formulation flag to indicate the thickness direction. Only valid for Isolid =14. 2
= 001
Reduced stress integration in t direction.
= 010 (Default)
Reduced stress integration in s direction.
= 100
Reduced stress integration in r direction.

(Integer)

  
Inpts Number of integration points.
= j
1 < j < 9 for Isolid =15
= ijk
2 < i,j,k < 9 for Isolid =14
= ijk
2 < i,k < 3, 2 < j < 9 for Isolid =16

(Integer)

Where:
i
Number of integration points in r direction.
j
Number of integration points in s direction.
k
Number of integration points in t direction.
  
Iint Thickness integration formulation. Only valid for Isolid =16.
= 1 (Default)
Gauss integration scheme.
= 2
Lobatto integration scheme.

(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)

  
Δ t min MathType@MTEF@5@5@+= feaagKart1ev2aqatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbbG8FasPYRqj0=yi0dXdbba9pGe9xq=JbbG8A8frFve9 Fve9Ff0dmeaabaqaciGacaGaaeqabaWaaeaaeaaakeaacaqGuoGaam iDamaaBaaaleaaciGGTbGaaiyAaiaac6gaaeqaaaaa@3B70@ Minimum time step

Default = 106 (Real)

 [ s ]

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 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.


      Figure 1.
      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. 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".

  3. 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.
  4. 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.
  5. 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.
  6. Numerical damping dn is only used in hourglass stress calculation for HSEPH (Isolid =15).
  7. Hourglass viscosity coefficient h must have a value between 0 and 0.15 and is not active with 8 integration point solids.
  8. 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.