/H3D/SHELL

Engine Keyword Generate H3D contour output results for /SHELL and /SH3N shell elements.

Format

/H3D/SHELL/Keyword3/Keyword4/Keyword5

#optional next line(s) that lists the parts to save results for.

part_ID₁ ... part_ID_N

Examples

# Stress tensor results for ply=1 and all integration points. The order of PLY and NPT does not matter.

/H3D/SHELL/TENS/STRESS/PLY=1/NPT=ALL
/H3D/SHELL/TENS/STRESS/NPT=ALL/PLY=1

# Stress tensor results for all integration points

/H3D/SHELL/TENS/STRESS/NPT=ALL

# Specific energy density results for only parts IDs 356 and 293.

/H3D/SHELL/ENER
356 293

# User variable #12 results for all integration points.

/H3D/SHELL/USER/NPT=ALL/UVAR=12

Definition

Field	Contents	SI Unit Example
`Keyword3`	Output types. 3
`Keyword4`	Output types. 3
`Keyword5`	Output types. 3
`part_ID`_N	Optional list of part IDs for which results will be output.

Comments

The syntax /H3D/ELEM/Keyword3/Keyword4/Keyword5 is also valid.
When PART IDs are listed after the /H3D/SHELL line the specified results will output only for those parts.

Output can be a, scalar, vector, or tensor as defined in the following tables.

Table 1. Scalar Output
Keyword3	Keyword4	Description
`ALPHA`	`PLY`= I or ALL `LAYER`= I or ALL	Shear angle alpha of material /MAT/LAW58 in degrees.
`AMS`		Elements using `AMS` timestep due to /DT/CST_AMS.
`BULK`		Artificial Viscosity
`DAM1`, `DAM2`, `DAM3`		Principal damage values in local orthotropic skew direction 1, 2 or 3 for materials LAW15 and LAW25.
`DAMA`	`MEMB` `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Maximum of damage over time of all /FAIL criteria acting on one material. Refer to the specific /FAIL law used for how damage is calculated.
`DAMA`	`TMAX`	Maximum of damage over time, integration points and failure models.
`DAMG`	`MEMB` `NPT`= I, ALL, LOWER or UPPER	Mean damage over thickness integration points (only for coupled damage models). 8
`DAMINI`	`PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Maximum damage initiation variable among all failure criteria using initiation variable before computing stress softening (/FAIL/INIEVO).
`DENS`		Density
`DOMAIN`		SPMD domain number of an element.
`DT`		Element timestep
`EINT`		Element internal energy
`ENER`		Specific energy density (internal energy divided by the element mass)
`ENER`	`TMAX`	Maximum specific energy density over time
`EPSD`		Equivalent strain rate
`EPSP`	`PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Plastic strain
`ERROR`	`THICK`	Estimated error on shell thickness
`FAIL`	`PLY`= I or ALL	Number of failed layers for /PROP/TYPE10, /PROP/TYPE11, /PROP/TYPE17, /PROP/TYPE51, /PCOMPP, /MAT/LAW15 and /MAT/LAW25. For the other property sets and material laws the values are: no failure =0 and element failed =1.
`FLDF`	`MEMB` `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	FLD damage factor indicator. 6
`FLDZ`	`MEMB` `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	FLD failure zone factor for the FLD failure model. 7 = 1 Loose metal = 2 High wrinkle = 3 Compression = 4 Safe = 5 Marginal = 6 Failure
`GROUP`		Internal group identifier
`HOURGLASS`		Hourglass Energy
`MASS`		Element mass
`MDS`		Automatic selection of user variable to output according to MDS law that is used. (1 value per user variable and per ply in case of stack and ply)
`MDS`	`MDS_VAR` = DEF or ALL (mandatory) `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	MDS user variables
`NL_EPSD`	`NPT`= I, ALL, LOWER or UPPER	Non-local plastic strain rate (only if /NONLOCAL/MAT is activated) 10
`NL_EPSP`	`NPT`= I, ALL, LOWER or UPPER	Non-local plastic strain (only if /NONLOCAL/MAT is activated) 10
`NXTF`	`MEMB` `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Instability factor of /FAIL/NXT failure model
`OFF`		Element status. Where the result output is: = -1 Element is not active (it is defined in an activated rigid body). = 0 Deleted element. Between 0 and 1 Under failure process. = 1 Active element.
`PEXT`		External pressure applied on shell element coming from /PLOAD, /LOAD/PFLUID, /LOAD/PBLAST or /LOAD/PRESSURE.
`PHI`	`MEMB` `PLY`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Angle between the element system and direction 1 orthotropy
`SIGEQ`		Equivalent stress based on a material’s yield criteria. Some examples of yield criteria are von Mises, Hill or Barlat.
`SIGEQ`	`TMAX`	Maximum equivalent stress based on a material’s yield criteria over time and integration points.
`SIGX`, `SIGY`, `SIGZ`, `SIGXY`, `SIGYZ`, `SIGZX`		Stress in specified direction
`TDEL`		Time at which element is deleted, due to failure defined using /FAIL criterion. Failure criteria built in materials is ignored.
`TEMP`		Temperature
`THICK`		Thickness
`THIN`		% thinning for shell.
`TSAIWU`	`PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Tsai Wu criterion for material /MAT/LAW15 (CHANG) and /MAT/LAW25 (COMPSH)
`USER`	`PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER `UVAR`= I or ALL	User material (/MAT/USERij) law output for user-defined variable `i`. Also, requests USR output for some Radioss material laws such as LAW58. USR1 output is requested using `UVAR`=1.
`VONM`		von Mises stress at neutral fiber
`VONM`	`TMAX`	Maximum von Mises stress at neutral fiber over time and integration points
`WPLA`	`PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Plastic work for /MAT/LAW15 (CHANG) and /MAT/LAW25 (COMPSH)

Table 2. Tensor Output
Keyword3	Keyword4	Keyword5	Description
`TENS`	`BSTRESS`	`ID`= n or ALL `MEMB` `BEND` `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I or ALL	Backstress tensor for material /MAT/LAW36 (n=1) and /MAT/LAW78 (n=1, 2 or 3) and /MAT/LAW87 (n=1, 2, 3 or 4). `ID`=-1 returns the sum of all backstress tensors available for the element.
	`EPSDOT`	`MEMB` `BEND` `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I or ALL	Strain rate tensor
	`STRAIN`	`MEMB` `BEND` `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I, ALL, LOWER or UPPER	Strain tensor
	`STRAIN`	`TMAX`	Strain tensor corresponding to the maximum principal strain (P1) over time and integration points. Strain tensor corresponding to the minimum principal strain (P3) over time and integration points.
	`STRAIN_ENG`	--	Infinitesimal total strain. Only one tensor per element.
	`STRESS`	`MEMB` `BEND` `PLY`= I or ALL `LAYER`= I or ALL `NPT`= I or ALL	Stress tensor
	`STRESS`	`TMAX`	Stress tensor corresponding to the maximum principal stress (P1) over time and integration points. Stress tensor corresponding to the minimum principal stress (P3) over time and integration points.

The output location in Keyword4 and Keyword5 can be defined via:

NPT

Integration points.

LAYER

Composite shell layer when using /PROP/TYPE11 (SH_SANDW), /PROP/TYPE10 (SH_COMP).

PLY

Composite shell ply when using, /PROP/TYPE19 (PLY) or /PLY.

MEMB

Generalized membrane stresses per element. Cannot be used with NPT, LAYER or PLY options.

BEND

Generalized bending stresses per element. Cannot be used with NPT, LAYER or PLY options.
Output can be requested for a specific location number (I), ALL, and in some case UPPER or LOWER. The output locations are separated by a / and can be in any order.
The values of FLD damage factor is equal to the ratio of the actual major principal strain value over the forming limit curve value:(1)
$F L D F = \frac{ε_{m a j o r}}{ε_{\lim}}$ $F L D F = \frac{ε_{m a j o r}}{ε_{\lim}}$

Where, $ε_{\lim}$ $ε_{\lim}$ is the major principal strain at failure limit from FLD diagram (fct_ID in /FAIL/FLD).

The FLD compares the $ε_{m a j o r}$ $ε_{m a j o r}$ and $ε_{\lim}$ $ε_{\lim}$ using the same $ε_{m i n o r}$ $ε_{m i n o r}$ .

Figure 1.

FLDF may be greater than 1, if the option /FAIL/FLD, Ifail_sh=4 is used. In this case, the damage factor is only calculated for post-processing and no elements are deleted.
The values of FLD zone index are defined as:

FLDZ=6

Failure

$ε_{m a j o r} > ε_{\lim}$ $ε_{m a j o r} > ε_{\lim}$

FLDZ=5

Marginal

$ε_{\lim} > ε_{m a j o r} > ε_{m \arg i n a l}$ $ε_{\lim} > ε_{m a j o r} > ε_{m \arg i n a l}$

FLDZ=4

Safe

$ε_{m \arg i n a l} > ε_{m a j o r} > | ε_{m i n o r} |$ $ε_{m \arg i n a l} > ε_{m a j o r} > | ε_{m i n o r} |$

FLDZ=3

Compression

$- ε_{m i n o r} > ε_{m a j o r} > - ε_{m i n o r} \cdot \frac{R_{a n i}}{1 + R_{a n i}}$ $- ε_{m i n o r} > ε_{m a j o r} > - ε_{m i n o r} \cdot \frac{R_{a n i}}{1 + R_{a n i}}$

FLDZ=2

High wrinkle

$- ε_{m i n o r} \cdot \frac{R_{a n i}}{1 + R_{a n i}} > ε_{m a j o r}$ $- ε_{m i n o r} \cdot \frac{R_{a n i}}{1 + R_{a n i}} > ε_{m a j o r}$

FLDZ=1

Loose metal

$ε_{m a j o r}^{2} + ε_{m i n o r}^{2} > F a c t o r_L o o s e m e t a l^{2}$ $ε_{m a j o r}^{2} + ε_{m i n o r}^{2} > F a c t o r_L o o s e m e t a l^{2}$

Figure 2.

Where,

fct_ID

Defined in /FAIL/FLD

$ε_{\lim}$ $ε_{\lim}$

Major strain as a limit from FLD diagram from fct_ID in /FAIL/FLD

$ε_{m i n o r}$ $ε_{m i n o r}$ and $ε_{m a j o r}$ $ε_{m a j o r}$

The minimum and maximum principal strains

R_ani

Average anisotropy factor defined in FLD input in /FAIL/FLD

$F a c t o r_M a r g i n a l$ $F a c t o r_M a r g i n a l$

Defined in FLD input in /FAIL/FLD

$F a c t o r_L o o s e m e t a l$ $F a c t o r_L o o s e m e t a l$

Defined in FLD input in /FAIL/FLD

(2)
$α = \arctan (- \frac{R_{a n i}}{1 + R_{a n i}})$ $α = \arctan (- \frac{R_{a n i}}{1 + R_{a n i}})$

I_marg

Defined in FLD input in /FAIL/FLD

If I_marg = 2, the marginal curve is defined by shifting the FLD curve with the constant value $F a c t o r_M a r g i n a l$ $F a c t o r_M a r g i n a l$ .(3)
$ε_{m \arg i n a l} = ε_{\lim} - F a c t o r_M a r g i n a l$ $ε_{m \arg i n a l} = ε_{\lim} - F a c t o r_M a r g i n a l$

If I_marg = 3, the marginal curve is defined as a factor of the $F a c t o r_M a r g i n a l$ $F a c t o r_M a r g i n a l$ .(4)
$ε_{m \arg i n a l} = ε_{\lim} (1 - F a c t o r_M a r g i n a l)$ $ε_{m \arg i n a l} = ε_{\lim} (1 - F a c t o r_M a r g i n a l)$
Option DAMG is only used with coupled damage models (/MAT/LAW72 or /FAIL/GURSON) to output damage over integration points. The damage variable is normalized by its critical value.
- For /MAT/LAW72(5)
  $D_{m g} = \frac{D}{D_{C}}$ $D_{m g} = \frac{D}{D_{C}}$
- For /FAIL/GURSON(6)
  $D_{m g} = \frac{f_{t}}{f_{F}}$ $D_{m g} = \frac{f_{t}}{f_{F}}$
When using global integration (N=0 in the shell property), Radioss always outputs the stress and strain only in the midplane (MEMB).
If /NONLOCAL/MAT option is activated, it is possible to output the regularized non-local plastic strain and its rate.
The damage initiation variable /H3D/SHELL/DAMINI is used with some failure criteria such as /FAIL/INIEVO, which first computes a damage initiation criterion before computing the stress softening damage variable, which can be plotted with /H3D/SHELL/DAMA.