# Eulerian method; basics

You may find examples and a tutorial at http://www.dynaexamples.com Eulerian fluids such as air or water are generally modeled using `*MAT_NULL`

and an accompanying equation-of-state (`*EOS_...`

).

For a case where there is only one Eulerian material, One approach would be to use solid element formulation 12 (single material with void) to model the Eulerian material and any empty cells around the Eulerian material into which that material may ultimately be transported. The empty cells (which typically overlay your Lagrangian parts) are identified using `*INITIAL_VOID`

. All the Eulerian parts (filled or void) should be given material/EOS properties of the Eulerian material.

A second approach (preferred) would be to use element formulation 11 (see next paragraph) and assign `*MAT_VACUUM`

to the void (empty) cells. In either case, use hexahedron (brick) elements for the Euler/ALE mesh and hourglass type 1. A reduced hourglass coefficient, e.g., .001, is recommended if the Eulerian material is a fluid.

For cases where there are multiple Eulerian materials, use solid formulation 11 (multi-material). For this, each Eulerian material must be assigned to a group using `*ALE_MULTI_MATERIAL_GROUP`

. Each part within a specific group has identical material properties.

**Eulerian meshing can be done using one of the following two approaches:**

- The initial mesh conforms to the material. In other words, there are no mixed (or partially filled) cells in the initial configuration. Mesh lines follow the outer contour of each Eulerian part.
- A simple orthogonal mesh may be constructed with no restriction that mesh lines follow the outer contour of each Eulerian part. The volume fraction of initially mixed cells must be prescribed via
`*INITIAL_VOLUME_FRACTION`

. Version 970 has a*geometry*option to`*INITIAL_VOLUME_FRACTION`

that automates the assignment of initial volume fractions to cells.

In either approach, there is no requirement that the Lagrangian nodes align with the Eulerian nodes. In your coupling definition (`*CONSTRAINED_LAGRANGE_IN_SOLID`

), you may have to increase `NQUAD`

if the structural mesh is coarser than the Eulerian mesh (in order to prevent *leakage* in the coupling). Your Lagrangian segment normals must point toward the Eulerian fluid (note you can reverse the normals using NORM). If you are coupling Lagrangian solids to the Eulerian fluid, `CTYPE`

should be set to 5 if erosion of the Lagrangian part occurs, otherwise set `CTYPE`

to 4. Set `MCOUP`

to 1 in cases where one of the Eulerian materials dominates the loads imparted to the Lagrangian structure, i.e. it's density is much higher than the other Eulerian materials. Typically `DIREC`

should be set to 2 when a penalty-based coupling is used. See euler.coupling for more recent information on coupling.

As an alternative to coupling (`*CONSTRAINED_LAGRANGE_IN_SOLID`

), you can, in some cases, merge (share) nodes at the interface between a Lagrangian part and an ALE part. The shared nodes will move as Lagrangian nodes. The interior of the ALE mesh must then be smoothed using one or a combination of smoothing algorithms (see `*CONTROL_ALE`

) and, if the situation warrants, `*ALE_SMOOTHING_CONSTRAINTS`

.

If you have a recent LS-PREPOST executable, you can view the Euler/ALE materials in a convenient manner by selecting Selpar > Fluid. The fluid part will be created and the Euler grid part appearance will be changed to edge. The fluid part can be fringed in Fcomp.

You can also view the Euler/ALE materials using Fcomp > misc > history variable

`1 = density`

`2 = volume fraction of 1st multi-material group (formulation 11) or single Eulerian material (formulation 12)`

`3 = volume fraction of 2nd multi-material group (formulation 11) etc.`

If n is the number of multi-material groups, then history variable #(n+2) is a component that identifies the various multi-material groups by assigning a value of 1.0 to those cells comprised predominantly of multi-material group 1, 2.0 to those cells comprised predominantly of multi-material group 2, and so on.

If `STRFLG`

is set to 1 (strains saved), the first six extra history variables for the Euler/ALE solid elements are strains. Thus in that case, density will be the 6+1=7th history variable.

It's sometimes clearer to view isosurfaces of Eulerian history variables rather than fringes (click on the Frin button and choose Isos).

**Notes:**

- The command
`*ALE_REFERENCE_SYSTEM(_OPTION)`

can be utilized in some situations to reduce the spatial extent of the initial Eulerian mesh. This command directs the Eulerian mesh to move through space in a prescribed manner rather than remaining fixed in space. - Air/structure interaction (non-HE applications): You may not need an ALE/Euler formulation to model air in such a case. Try modeling the air with regular Lagrangian elements (ELFORM 1) and merge the solid air elements to the structure.
`*MAT_NULL`

with`*EOS`

is probably a better bet for air than`*MAT_ACOUSTIC`

.

For air to be modeled with ALE/Euler elements, the motion of the structure needs to be significant relative to the ALE elm size modeling the air - i.e. it has to push into the air a good distance to generate the pulse.

jpd 8/2002 revised 11/5/02 revised 11/14/02 revised 1/6/03 revised 6/2003 revised 12/2003