# Define composites

**A. Transverse shear strain in composites**

By default, shells in LS-DYNA make the assumption of uniform transverse shear strain. This assumption is invalid for foam core composites or any stackup with lamina comprised of different materials with largely varying stiffness.

**To correctly calculate the stiffness of sandwich composites (particularly foam cores) using shells, laminate theory must be invoked in LS-DYNA verion 960 by any one of several means:**

- Use
`MAT_22,54, or 55`

with`LAMSHT=1`

on optional card 2 of`*CONTROL_SHELL`

- Use
`MAT_114`

, a plasticity model patterned after`MAT_24`

. - Use
`MAT_116`

, a resultant layup-theory model.

**B. Modeling multi-layer composites**

There are several options for modeling layered composites with shell elements. The simplest and least general is to use the BETA option of `*SECTION_SHELL`

to define the material direction for each integration point through the element thickness. A user-defined integration rule should also be used to control the layer thicknesses. (see `IRID`

of `*SECTION_SHELL`

, and `*INTEGRATION_SHELL`

).

If a composite is made up layers of different materials, a more general composite can be modeled by specifying a different part ID for each integration point (see `*INTEGRATION_SHELL`

). Each part can refer to a different material model with the restriction that all materials must be of the same type. For example, you could specify an element with one layer of material type 2 using `Ea = 10`

, `Eb = 1`

, and another layer of material type 2 with `Ea = 3`

, `Eb = 3`

, where Ea and Eb are the Young's modulus in the *a* and *b* directions. This method allows different material constants to be used in the different layers, but still does not allow completely general mixing of material types in a single shell element.

In version 970, the PID in `*INTEGRATION_SHELL`

(if specified) points to a part but only the material data from that part is used. The section data comes from the part referenced by the `*ELEMENT_SHELL`

command. Notice that there is a much more intuitive approach in v. 971.

Revision 894 of V971 allows for different material types to be used in a user-defined shell integration rule. For now (9/2003), some materials, notably rubbers, are excluded from this capability. It should work for plasticity models and orthotropic materials.

V970 does NOT have the capability to mix material types in a single integration rule. It would be fortuitous if a mixed material model ran to completion using V970. The results would not be physical. A laborious approach that could be taken in versions preceding V971,r894 would be to model the section with multiple elements, one element for each material type in the composite. The elements should all be given a thickness equal to the total composite thickness and should all share the same nodes, so they would appear to all lie in the same space when viewed in a preprocessor or postprocessor. However, in order to obtain the correct membrane and bending stiffness for the whole composite element, define a separate integration rule for each element in the composite with appropriate weights and through thickness locations. A simple example of a sandwich type composite with one material in the middle and another on the top and bottom surface might have integration rules like this.

The middle material could have 2 integration points with weights and thickness coordinates of

`Wf1 = 0.25, S1 = -0.25`

`Wf2 = 0.25, S2 = +0.25`

The surface material could have 2 integration points with weights and thickness coordinates of

`Wf1 = 0.25, S1 = -0.75`

`Wf2 = 0.25, S2 = +0.75`

In this example, Wf1 is the weight factor for integration point 1, and S1 is the thickness direction coordinate of integration point 1 etc. The correct stiffness is achieved so long as the total weight of all elements is equal to 1, and the thickness coordinates are defined such the integration points are at the middle center of each layer. This method has complete freedom of material type for each layer. It seems like a great idea, but . . .

LS-DYNA has built in protection to prevent the input of weights that don't add up to 1. If you try the example, it converts the weights at all integration points to 0.5 so that they add up to one for each element. Fortunately, there is a trick to get around this protection. The idea is to reduce the thickness of elements accordingly so that the correct membrane stiffness is achieved for each material. In other words, each element should have a thickness equal to the actual summed thickness of layers of that material. In the example, the element thickness of both elements should be reduced to one half the total composite thickness. Then to achieve the correct bending stiffness for the composite, the thickness coordinates for each integration point should be increased accordingly. In the example, since each element has been reduce to half the composite thickness, the thickness coordinates should be doubled, so `S1 = -0.5`

, `S2 = +0.5`

for the middle material, and `S1 = -1.5`

, `S2 = +1.5`

for the surface material. Notice that this violates the usual restriction the thickness coordinates should be in the range of -1 to +1. However, it works because LS-DYNA does not enforce this rule.

In this simple example, each of the 4 material layers has a thickness of 1/4 of the total element thickness. However, there is absolutely no restriction on the number of layers, thickness of layers, or material of the layers using this method.

**The only rules that should be followed to achieve correct stiffness of the overall composite element are:**

- The sum of individual element thicknesses should equal the total composite thickness.
- The thickness coordinates for each integration point should be multiplied by the total composite thickness and divided by the corresponding element thickness.

If multi-element method is used, care should be taken if the composite is to be checked for contact. Only one of the elements making up the composite should be checked for contact since all element share the same nodes. However, the element thickness will be less than the composite thickness, so it may be desirable to directly prescribe the thickness for contact (see `SST`

,`MST`

on `*CONTACT`

) if using a contact type where element thickness is taken into account.

lpb, jpd revised 9/10/03