Post-processing

Active strain output in T01 file and ANIM file.

Using shell elements, I asked for strain Time History output (RunnameT01) and Animation files, but the values remain equal to zero; why?

The strain tensor is not computed by default; it must be asked for in the Radioss input file (Runname_0000.rad) by setting flag I_strain (flag to compute strains for post-processing) to 1 in option /DEF_SHELL or in the shell property set.

On the contrary, the strain tensor is always computed and available for /MAT/LAW25 (COMPSH) and /MAT/LAW27 (PLAS_BRIT).

Element strain rate animation output with EPSD.

/ANIM/ELEM, BRICK or /SHELL/EPSD and Variable EPSD for a group of shells or 3-node shells for Time History: I asked for strain rate output but the values remain equal to zero into post-processors; why?

Strain rate filtering needs to be activated (F_smooth=1), but it is available for most material laws but not for all.

It is not possible to get these outputs if the material law does not allow filtering (or “smooth”) the strain rate. On the contrary, using F_smooth =1 and F_cut =1.E+30 will allow for all these laws to get these outputs without filtering the strain rate (indeed, filtering is activated but the cut-off frequency is so high that no filtering happens at all).

In certain cases, the outputs are also available even if strain rate filtering had not been asked for (F_smooth =0).

This variable EPSD is available for both Animations and Time History in case of shell elements; it is only available for Animations in case of solid elements.

Output to ANIM or Time History files of strain rate for shell elements.

Table 1. 3- and 4-Node SHELL Elements
Material Law	Available with V51?	Available with V90?
LAW2	In any case	In any case
LAW15	If `F`_smooth=1	If `F`_smooth=1
LAW25	If `F`_smooth=1	If `F`_smooth=1
LAW27	If `F`_smooth=1	If `F`_smooth=1
LAW36	In any case	In any case
LAW44	If `F`_smooth=1	If `F`_smooth=1
LAW48	If `F`_smooth=1	If `F`_smooth=1

Output to ANIM files of strain rate for solid elements.

Table 2. SOLID Elements
Material Law	Available with V51?	Available with V90?
LAW2	In any case	In any case
LAW36	In any case	In any case
LAW44	If `F`_smooth=1	If `F`_smooth=1
LAW48	If `F`_smooth=1	If `F`_smooth=1
LAW50	If `F`_smooth=1	If `F`_smooth=1

Shell stress of SIGX, SIGY, and VONM in Animation.

What are the stresses SIGX, SIGY, and VONM in Animation files if I use integration points for the shells?

The stresses SIGX, SIGY… in Animation files represent the mean stresses through the thickness of the shell element. The VONM stress represents the von Mises criteria applied to these mean stresses SIGX, SIGY… In the same way the stresses F1, F2, F12, Q1 and Q2 given in Time History correspond to these mean stresses.

These mean stresses are computed by summation of the stresses at each integration point, averaged by the integration weights (refer to Integration Points Throughout the Thickness in the Radioss Theory Manual). They are used for the internal forces calculation.(1)

σ = \sum_{k = 1}^{n} w_{k} \cdot σ_{k}

EPSP animation output for different element type.

Which value is output when using /ANIM/ELEM/EPSP when using different element type?

/ANIM/ELEM/EPSP output the plastic strain of element.

For Bricks
It is the mean value calculated using relative volumes of the different integration points.
For Quads
/ANIM/ELEM/EPSP is not available for Quad element. No value will be output.
For Shells
- The plastic strain at the middle integration point is output. When an even number of integration points are requested, then the N/2 + 1 integration point is output.
- For 4-node shell element with I_shell=12 (QBAT) element formulation, the mean value of EPSP of the 4 in-plane gauss points of the middle integration point is output.
- It is recommended to use /ANIM/SHELL/EPSP/Keyword4, to get the plastic strain results at the upper and lower integration points. Especially in bending, the plastic strain in mid-layer will be less than the outer integration points.
For Beams
It is the mean value calculated using the relative areas of the different integration points.

What is the output to Animation files with /ANIM/ … /ENER?

The specific energy per mass unit.

What is the output to Animation files with /ANIM/ … /HOUR?

The Hourglass energy per mass unit.

QEPH element energy output.

Using shell elements with QEPH formulation (I_shell=24), the hourglass energy of the part and the subset are not equal to zero in Time History; why?

When looking to the SUBSET or the PART in Time History, the hourglass energy is not zero.

This is because energy absorbed due to the numerical damping is output there. This means, in output the place of hourglass energy has been used to present this viscous energy.

The viscous energy is related to coefficient dn for shell property which using QEPH (I_shell =24) and QBAT and DKT18 (I_shell =12 or I_sh3n =30).

The energy corresponding to the physical stabilization of hourglass is counted as internal energy for this formulation.

Animation GZIP file readability.

Using /ANIM/GZIP the Animation files are not readable; why?

This option uses the Gnu tool: GZIP which is normally available on Linux. Verify that it is installed correctly on the machine Radioss is running on Windows, GZIP is included with the Altair Simulation installation.

Difference of EPSP output with /ANIM and /OUTP.

What is the difference between /ANIM and /OUTP for EPSP output?

Runname_nnnn.sty files contain both membrane and maximum (over the integration points through the thickness) values; whereas, Annn files contain only membrane value.

Animation file generation control during running.

Is it possible to get more (or less) Animation files while a computation is running?

Yes it is possible to write an Animation file by writing a control file in the data directory.

For the run number nn (/RUN/Runname/nn in the Radioss Engine input file), you have to write the file Runname_nn_0000_[C].rst with the process /ANIM in it.

Radioss Engine writes an Animation file at this time.

The other options available with control files are described in the Control File (C-File) file.

In order to change the Animation files writing frequency, you have to stop your Radioss computation while writing a RESTART file, by using a control file (option /STOP). Then you can chain a second run with a different frequency for the Animation files writing.

Display eroded element.

How can I plot deleted elements to understand the propagation of a fracture?

Select Preferences > Option > Visualization menu in HyperView to display Eroded Elements.

This will help you to understand the propagation of a fracture.

Shell stress tensor output in animation.

How is the generalized stress tensor /ANIM/SHELL/TENS/MEMB and /ANIM/SHELL/TENS/BEND computed?

The generalized membrane and bending stress tensor is computed for each plane (layer) according the deformation, the bending behavior of the shell elements, and the material law.

For the shell property /PROP/TYPE1 (SHELL) or /PROP/TYPE9 (SH_ORTH):

For global integration, (N=0)
The exact computation is done from the generalized strain tensor and the result will correspond to:(2)
$σ_{g} = {\begin{matrix} M e m b r a n e \begin{matrix} \end{matrix} s t r e s s = \frac{1}{t} \int_{- t / 2}^{+ t / 2} σ d z \\ B e n d i n g \begin{matrix} \end{matrix} s t r e s s = \frac{1}{t^{2}} \int_{- t / 2}^{+ t / 2} σ z d z \end{matrix}}$

For multiple integration points through the thickness (N > 0)

The generalized stress (

σ_{g}

) is computed for each plane (layer) and integrated according to the defined weights, which includes the position through the thickness and the relative thickness.(3)

σ_{g} = {\begin{matrix} M e m b r a n e \begin{matrix}  \end{matrix} s t r e s s = \sum_{i = 1}^{N} w_{i}^{N} \cdot σ_{i} \\ B e n d i n g \begin{matrix}  \end{matrix} s t r e s s = \sum_{i = 1}^{N} w_{i}^{M} \cdot σ_{i} \end{matrix}}

Weight for membrane stress tensor (

w_{i}^{N}

) computation.

#point(s)	$w_{i}^{N}$
1	1.0000
2	0.5000	0.5000
3	0.2500	0.5000	0.2500
4	0.1667	0.3333	0.3333	0.1667
5	0.1250	0.2500	0.2500	0.2500	0.1250
6	0.1000	0.2000	0.2000	0.2000	0.2000	0.1000
7	0.0833	0.1667	0.1667	0.1667	0.1667	0.1667	0.0833
8	0.0714	0.1429	0.1429	0.1429	0.1429	0.1429	0.1429	0.0714
9	0.0625	0.1250	0.1250	0.1250	0.1250	0.1250	0.1250	0.1250	0.0625
10	0.0556	0.1111	0.1111	0.1111	0.1111	0.1111	0.1111	0.1111	0.1111	0.0556

Weight for bending stress tensor (

w_{i}^{M}

) computation.

#point(s)	$w_{i}^{M}$
1	0.0000
2	-0.0833	0.0833
3	-0.0833	0.0000	0.0833
4	-0.0648	-0.0556	0.0556	0.0648
5	-0.0521	-0.0625	0.0000	0.0625	0.0521
6	-0.0433	-0.0600	-0.0200	0.0200	0.0600	0.0433
7	-0.0370	-0.0556	-0.0278	0.0000	0.0278	0.0556	0.03
8	-0.0323	-0.0510	-0.0306	-0.0102	0.0102	0.0306	0.0510	0.0323
9	-0.0286	-0.0469	-0.0313	-0.0156	0.0000	0.0156	0.0313	0.0469	0.0286
10	-0.0257	-0.0432	-0.0309	-0.0185	-0.0062	0.0062	0.0185	0.0309	0.0432	0.0257

For the shell property defined by layers, /PROP/TYPE10 (SH_COMP), /PROP/TYPE11 (SH_SANDW), /PROP/TYPE17 (STACK).

The generalized stress (

σ_{g}

) is computed for each layer and integrated according to the relative layer thickness (layer thickness/total thickness) and the position on the layer z (isotropic value of z: -0.5 < z < 0.5).(4)

σ_{g} = {\begin{matrix} M e m b r a n e \begin{matrix}  \end{matrix} s t r e s s = \sum_{i = 1}^{N} \frac{t h i c k_{i}}{t h i c k} \cdot σ_{i} \\ B e n d i n g \begin{matrix}  \end{matrix} s t r e s s = \sum_{i = 1}^{N} \frac{t h i c k_{i}}{t h i c k} \cdot z_{i} \cdot σ_{i} \end{matrix}}

Note:

N=1 defines a membrane element. The bending stress tensor is zero.
For fully integrated element shells (I_shell=12), the stress tensor output for each plane (layer) is the average value of the 4 Gauss points.
For the property /PROP/TYPE51, several integration points through the thickness can be defined for each layer. The generalized stress computation will be done according to the shell property defined by the layers with different height through the thickness (z) using the layer position and the selected distribution through the layer formulation (/PROP/TYPE51).

Integration points through shell thickness:

	Number of Integration Points	Distribution of Integration Points	Number of Layer
/PROP/TYPE1	`N` ( $0 \leq N \leq 100$ )	Lobatto integration scheme	-
/PROP/TYPE9	`N` ( $1 \leq N \leq 100$ )	Lobatto integration scheme	-
/PROP/TYPE10	1 per layer	Middle of layer	`N` ( $0 \leq N \leq 100$ )
/PROP/TYPE11	1 per layer	Middle of layer	`N` ( $0 \leq N \leq 100$ )
/PROP/TYPE16	1 per layer	Middle of layer	`N` ( $0 \leq N \leq 100$ )
/PROP/TYPE17	`Npt_ply` in /PROP/TYPE19 ( $1 \leq N p t_p l y \leq 9$ )	Uniform integration scheme	`Pply_IDi` ( $1 \leq P p l y_I D i \leq n$ )
/PROP/TYPE51	`Npt_ply` in /PROP/TYPE19 ( $1 \leq N p t_p l y \leq 9$	`I`_int=1: Uniform integration scheme `I`_int=2: Gauss integration scheme	`Pply_IDi` ( $1 \leq P p l y_I D i \leq n$ )

For the position and weight of the Gauss integration scheme and Lobatto integration scheme, refer to Integration Points Throughout the Thickness in the Theory Manual.

Stress or strain outputs for LAW38 and LAW70.

The type stress and strain output, engineering or true, for LAW38 and LAW70 depend on the value of I_smstr defined in /PROP.

For LAW70, small strain (I_smstr=1 or 11) is recommended so the stress and strain input and output are engineering.

For LAW38, large strain (I_smstr=4 or 10) is used. In this case, the stress is Cauchy stress (true stress) and strain is the total true strain for Left Cauchy-Green. The engineering stress/strain input curve will be translated to the true stress/strain automatically.

With certain options in Radioss (as in, /DT/BRICK/CST), the element formulation might be switched to the small strain formulation during the run. In this case, for LAW38, the output consists of both true and engineering. Initially, the stress and strain accumulated are true, but after the switch to small strain by the element, engineering stress and strain accumulated.