Property and Elements

I have a problem using /PROP/TYPE16 (SH_FABR) for fabric shell. What is the meaning of ERROR ID: 28

I defined Thick in global thickness as 0.93, then I set three layers each 0.31 mm thickness.

ERROR ID : 28
** ERROR IN LAYERED SHELL SET
FOR LAYERED SHELL PID 15 :
NUMBER OF LAYERS MUST BE LOWER OR EQUAL TO 1

WARNING ID : 29
** WARNING WITH COMPOSITE SHELL THICKNESS
SHELL THICKNESS DISCREPENCY WITH
SUM OF LAYER THICKNESSES IS 67 PERCENT

     LAYER   1
           ANGLE (DIR 1,PROJ(VECT / SHELL) .= 0.000000000000
           ANGLE (DIR 1,DIR 2) . . . . . . .= 90.00000000000
           THICKNESS . . . . . . . . . . . .= 0.9300000000000
           POSITION. . . . . . . . . . . . .= 0.000000000000
           MATERIAL NUMBER . . . . . . . . .= 2

In Radioss versions before 2017, this error means the number of layers defined for /PROP/TYPE16 was set to N>1. To fix this issue, set N=1.

Which strain formulations are available for connection element with /PROP/CONNECT?

/PROP/CONNECT is used only for /MAT/LAW59 (CONNECT) and /MAT/LAW83. This element formulation is based on relative elongation of element in normal and shear direction. This allows avoiding the dependence of element time step from element height. Element height can be even equal to 0. Note that material stiffness is specified in normal and in shear direction. Material has no stiffness in lateral direction. Therefore, it is always advised to couple nodes of LAW59 elements to some Lagrange components either directly or through a tied contact.

The parameter I_smstr in /PROP/TYPE43 (CONNECT) specifies how the nodal forces are calculated from stresses.

For I_smstr=4 use the actual middle area of the element and for I_smstr=1 use initial middle area. This is implemented in order to avoid time step drop, when LAW59 or LAW83 element separates from master surface (due to the failure of master surface elements) and it starts to expand laterally.

How does Radioss calculate layer thickness and layer position in /PROP/TYPE11 and /PROP/TYPE16?

In these two properties, options Thick, ti and I_pos will affect the layer thickness and layer position.

I_pos = 0:

Layer positions Zi are automatically calculated with regard to layer thicknesses.

If the sum of layer thickness is different from the input value Thick, a warning message is displayed. Then Radioss adjusts the layer thickness and layer position.

Example 1

Shell thickness Thick (1.8) is not equal to the sum of layer thickness (0.5+0.6+0.5=1.6) in input.

During the computation, Radioss takes the sum of input layer thickness (1.6) to adjust each layer thickness with $\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{\sum ti\_input}$ . So that the adjusted sum of layer thickness is in respect to shell thickness Thick (1.8).

The position of each layer is also adjusted regarding to the new layer thickness.

Figure 1.

The Adjusted layer thickness is calculated:

Adjusted Layer Thickness	Layer Position
$\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{\sum ti\_input}$
$\text{t}1=0.5\ast \frac{1.8}{1.6}=0.5625$	$\text{Z}1=-\left(\frac{\text{Thick}}{2}-\frac{t1}{2}\right)=-\left(\frac{1.8}{2}-\frac{0.5625}{2}\right)=-0.61875$
$\text{t}2=0.6\ast \frac{1.8}{1.6}=0.675$	$Z1=0$
$\text{t}3=0.5\ast \frac{1.8}{1.6}=0.5625$	$\text{Z}3=\frac{\text{Thick}}{2}-\frac{t3}{2}=\frac{1.8}{2}-\frac{0.5625}{2}=0.61875$

Figure 2.

Note: The local Z-axis defines the position of middle of the thickness shell. Since the Zi values are real layer positions in the local Z axis, the negative and positive values of Zi are allowed.

Figure 3.

I_pos= 1:

All layer positions Zi in the element thickness MUST be user-defined.

• If multiple layers may have the same special position (overlapped), a warning message is displayed. In this case, the layer thickness will also be adjusted.

Example 2

If I_pos=1 but layer position Zi leave as default (set to 0). In this case, layers are all in the same position and overlap each other.

During the computation, Radioss takes the thickness of the thickest layer (0.6) to adjust each layer thickness with $\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{Thickness of thickest layer}$ .

The position of each layer will not be adjusted.

Figure 4.

The Adjusted layer thickness is calculated:

Adjusted Layer Thickness	Layer Position
$\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{Thickness of thickest layer}$
$\text{t}1=0.5\ast \frac{1.8}{0.6}=1.5$	$Z1=0$
$\text{t}2=0.6\ast \frac{1.8}{0.6}=1.8$	$Z1=0$
$\text{t}3=0.5\ast \frac{1.8}{0.6}=1.5$	$Z1=0$

Figure 5.

• If multiple layers may have a small overlap or a gap, a warning message is displayed. In this case, the layer thickness and layer position will be also adjusted.

Example 3

If I_pos=1 but layers have a small overlap, due to the user-defined Zi. In this case, layers thickness and layer position will be adjusted.

During the computation, Radioss calculates the distance between upper and lower surfaces of layers:(1)

$$\text{Dist}=\left|\left(\text{Z}1+\frac{t1}{2}\right)+\left(\text{Z}3+\frac{t3}{2}\right)\right|=\left|\left(0.5+\frac{0.6}{2}\right)+\left(0.5+\frac{0.6}{2}\right)\right|=1.6$$

And takes this distance to adjust each layer thickness with $\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{Dist}$ .

Figure 6.

The Adjusted layer thickness is calculated:

Adjusted Layer Thickness	Layer Position
$\text{ti}=\text{ti}\_\text{input}\ast \frac{Thick}{Dist}$
$\text{t}1=0.6\ast \frac{1.8}{1.6}=0.675$	$\text{Z}1=\frac{\text{Thick}}{2}-\frac{t1}{2}=\frac{1.8}{2}-\frac{0.675}{2}=0.5625$
$\text{t}2=0.6\ast \frac{1.8}{1.6}=0.675$
$\text{t}3=0.6\ast \frac{1.8}{1.6}=0.675$	$\text{Z}3=-\left(\frac{\text{Thick}}{2}-\frac{t3}{2}\right)=-\left(\frac{1.8}{2}-\frac{0.675}{2}\right)=-0.5625$

Note: The local Z-axis defines the position of middle of the thickness shell. Since the Zi is user-defined, the layers are stacked according to the user definition.

Figure 7.

The run stopped with the message: "Zero or Negative Volume", when solid elements are used with I_smstr=2 and /DT/BRICK/CST; is this normal?

I_smstr =1, 2 , 3 and 11 (Small strain formulation) are only available for these 4-node and 8-node elements: I_solid = 1, 2, 14, 17, or 24 (standard, HA8, and HEPH solids).

"Zero or Negative Volume"

In order to use this small strain formulation with 8 integration points solid elements, use the HA8 solid formulation which is available as of Radioss V44.

When using this formulation, set I_solid =14 with I_npts =222 (corresponding to I_solid =222 in input format 44). Also set I_cpre =1 for elastic or visco-elastic material law, and I_cpre =2 for elasto-plastic laws.

I used solid elements and several integration points, and Starter the following error message appears, while the element seems to be well-defined: ** ERROR: ZERO OR NEGATIVE 3D SOLID VOLUME, is this normal?

** ERROR:  ZERO OR NEGATIVE 3D SOLID VOLUME
ZERO OR NEGATIVE VOLUME 3D-ELEMENT NB 1

Figure 8.

In Figure 8, the volume of the element is positive, but the sub-volume associated to one integration point is negative.

The solid is decomposed into sub-volumes associated to each integration point. If the element is badly warped, one sub-volume could be negative.

How many integration points should be used in the thickness of shell elements?

If only one integration point is used, a membrane only behavior will be obtained (except with LAW1, up to V44). Some materials, such as fabric, can justify such a choice (no bending strength).

In case of an elastic behavior, one gets the exact solution from three integration points – that is to say that the bending moments are exactly integrated through the thickness of the shell – and it is not necessary to use more integration points.

In case of a plastic behavior, the bending moments are not integrated exactly. Using more integration points, the solution becomes more accurate; so it is recommended to use five integration points.

Figure 9.

With shell elements using the same material law, but different types of properties (while keeping the same number of integration points), I do not get the same results; why?

The integration scheme which is used for property types 1 and 9 (relative to isotropic shells through the thickness) sets the integration points and weights in order to integrate exactly the bending moments in the elastic case (from three integration points since for one integration point, no bending moments are computed).

The integration scheme which is used for property types 10 and 11 is a step-by-step integration scheme and uses integration points at the center of each layer, and weights which correspond to the relative thickness of each layer. So the integration scheme is not the same one.

An error relatively important can occur in the elastic field, when there are a few layers or large differences on the thicknesses of the layers. One way to work around this problem is to subdivide the thicker layers. But it is generally not well-suited in case of modeling the failure of the layers.

Figure 10.

When is it better to use QEPH shells instead of Belytschko shells?

QEPH shells are more accurate for elastic or elasto-plastic loads, whatever the loading type - quasi-static or dynamic; but they are not recommended with anisotropic and orthotropic material laws.

QEPH shells will give better results if the mesh is fine enough. In case of a coarse mesh, this formulation will be too stiff and some local buckling phenomena could be missed. In case of a coarse mesh, the Belytschko shells often give better results.

QEPH/HEPH is compatible with orthotropic properties/materials since v14.0.

I used solid elements and the run stopped before the end time, with the message: "Zero or Negative Volume": How can this problem be solved?

This happens when solid elements are very deformed and their characteristic length goes to 0. You may notice in the output file before getting this error message, the time step of the element written into the message drops down.

In case of large strain formulation, the time step of an element goes to 0 when the element is compressed. In a mathematical way, the element cannot reverse its orientation since its stiffness increases to an infinite value; but due to numerical accuracy, the element may go to reverse its orientation.

Figure 11.

In order to solve the problem of both the drop in cycle time step and subsequent termination of the run due to a negative volume, you might first check that the material used is well-suited to the physics which is represented. Then switch the elements to small strain formulation. This is done as follows:

In the Radioss Starter input file (Runname_0000.rad), use I_smstr =2 in the solid property or in the option /DEF_SOLID; in Radioss Engine file (Runname_0001.rad) use the option /DT/BRICK/CST which will set the time step value $\text{Δ}{T}_{\min }$ at which the solid elements will switch to small strain.

This means that the solid elements using I_smstr =2 will use large strain formulation while their time step remains greater than $\text{Δ}{T}_{\min }$ , and will then switch to small strain formulation.

Their volume will then remain constant and the element can even reverse its orientation. The drop of their time step normally stops except for some materials, especially viscous materials.

What is the meaning of ERROR ID: 174 SPH?

MESSAGE ID :          174
** ERROR : NULL DIAMETER FOR SPH PARTICLE ID=52032255

This message means that an SPH particle is compressed so much that its diameter is zero which causes this error.

Most of the time, this is due to an input error, such as entering information in the wrong units. It is recommended to check the consistency between mass, density, diameter and particle pitch. Also, review that the material input is correct.

To see the particle diameter, review the “Diameter” animation contour is always available for the particles.