# Negative volume in soft materials

In materials that undergo extremely large deformations, such as soft foams, an element may become so distorted that the volume of the element is calculated as negative. This may occur without the material reaching a failure criterion. There is an inherent limit to how much deformation a Lagrangian mesh can accommodate without some sort of mesh smoothing or remeshing taking place. A negative volume calculation in LS-DYNA will cause the calculation to terminate unless `ERODE`

in `*CONTROL_TIMESTEP`

is set to 1 and `DTMIN`

in `*CONTROL_TERMINATION`

is set to any nonzero value in which case the offending element is deleted and the calculation continues (in most cases). Even with `ERODE`

and `DTMIN`

set as described, a negative volume may cause an error termination.

**Some approaches that can help to overcome negative volumes include the following:**

- Simply stiffen up the material stress-strain curve at large strains. This approach can be quite effective.
- Sometimes tailoring the initial mesh to accomodate a particular deformation field will prevent formation of negative volumes. Again, negative volumes are generally only an issue for very severe deformation problems and typically occur only in soft materials like foam.
- Reduce the timestep scale factor. The default of 0.9 may not be sufficient to prevent numerical instabilities.
- Avoid fully-integrated solids (formulations 2 and 3) which tend to be less stable in situations involving large deformation or distortion. (The fully integrated element is less robust than a 1-point element when deformation is large because a negative Jacobian can occur at one of the integration points while the element as a whole maintains a positive volume. The calculation with fully integrated element will therefore terminate with a negative Jacobian much sooner than will a 1-point element.)
- Use the default element formulation (1 point solid) with type 4 or 5 hourglass control (will stiffen response).Preferred hourglass formulations for foams are
- Type 6 with hourglass coef = 0.1 if low velocity impact
- Type 2 or 3 with hourglass coef. = 0.1 if high velocity impact.

- The hourglass type and hourglass coefficient may warrant modification based on observed hourglass modes and on reported hourglass energy in matsum

- Model the foam with tetrahedral elements using solid element formulation 10 although this approach may give an overly stiff response.
- Increase the
`DAMP`

parameter (foam model 57) to the maximum recommended value of 0.5. - Use optional card B of
`*CONTACT`

to turn shooting node logic off for contacts involving foam. - Use
`*CONTACT_INTERIOR`

. A part set defines the parts to be treated by`*CONTACT_INTERIOR`

. Attribute 4 (`DA4`

= 5th field of Card 1) of the part set defines the`TYPE`

of`*CONTACT_INTERIOR`

used. The default`TYPE`

is 1 which is recommended for uniform compression. In version 970, solid formulation 1 elements can be assigned`TYPE=2`

which treats combined modes of shear and compression. - If
`*MAT_126`

is used, try`ELFORM = 0`

. - Try EFG formulation (
`*SECTION_SOLID_EFG`

). Use only where deformations are severe as this formulation is very expensive. Use only with hex elements.

jpd