Result Mapping

Purpose:

This interface is used for mapping *INITIAL_STRESS, including plastic strain, shell thickness and history variables, from one part to another geometrically overlapping part.

Detailed description for each map option.

Shell to Solid mapping. The coordinate for each solid element integration point will be projected on to the closest shell element. This will be the shell element from which the results will be mapped from.

In order to map from a shell to solid element part, the user have to specify the two topological sides on the solid part(s), which corresponds to the upper and lower surface of the shell elements. These are called "Side 1" and "Side 2" in the interface below.

A parametric position beween "Side 1" and "Side 2" will then be computed for each integration point in the solid elements. Data from the through-thickness shell integration point which best matches this parametric position will be selected for mapping of the results.

If the shell has four in-plane result values, an inter- or extrapolated value will be computed at the point on the shell which is closest to the solid element integration point. This inter/extrapolated value will be assigned to the solid element integration point. Meaning that it can actually become larger than the largest of the four shell in-plane values, or smaller than the smallest. Plastic strain will however never be extrapolated to a negative value. Only stress and plastic strain are interpolated, not history variables. History variable values will be assigned from the closest integration point.

Solid to Solid mapping. The integration point to map to can either be inside or outside the solid elements with results. If it's outside, the closest point on the closest element will be found. The stresses and plastic strain will be inter/extra-polated to this location and the value will be assigned to the integration point. History variable values will be assigned from the closest integration point, i.e. they will not be inter- or extrapolated.

Shell to Shell mapping. The number of integration points specified on SECTION_SHELL will be used when deciding how many through-thickness integration points will be used for the generated *INITIAL_STRESS keyword. Much like Shell to Solid mapping, the closest parametric coordinate for the through-thickness integration point will be used for assigning the values. In-plane inter/extra-polation is done for the stress and plastic strain. Plastic strain will however never be extrapolated to a negative value. History variable values will be assigned from the closest integration point.

Solid to Shell mapping. "Side 1" and "Side 2" needs to be defined for the solid part(s). The *INITIAL_STRESS and thickness can be mapped in two different ways, A and B:

A: If leaving "Target IPs" field empty, the initial_stress results will be mapped to the integration points specified by the *SECTION_SHELL of the shell part and thickness will be applied to *ELEMENT_SHELL_THICKNESS. For each integration point in the shell, the closest points on "Side 1" and "Side 2" will be found. The thickness of the shell will be set to the distance between these two points. The stress will be extracted from the parametric position between "Side 1" and "Side 2" corresponding to the parametric coordinate of the through-thickness shell integration point.

B: Mapping results from a multi-part layered (composite) solid to ELEMENT_SHELL_COMPOSITE can be activated by specifying a list of through-thickness integration point number(s) in the "Target IPs" text field. The thickness between "Side 1" and "Side 2" will be evenly distributed to the specified integration points. The stress results will be extracted from the parametric position between "Side 1" and "Side 2" corresponding to an even distributed of the specified integration points.
In-plane inter/extra-polation is done for the stress and plastic strain. Plastic strain will however not be extrapolated to a negative value. History variable values will be assigned from the closest integration point.
For example, if the solid structure is composed of three parts as a traditional sandwich structure with stiff outer skins and a softer core, the mapping to the *ELEMENT_SHELL_COMPOSITE must be made in three steps. The option "Fully integrated"must remain the same for all three mappings as the number of in-plane integration points must remain the same in a *INITIAL_STRESS_SHELL keyword. "Target IPs" have to be specified for the three mappings as well to get a mapping to *ELEMENT_SHELL_COMPOSITE. The target integration points are numbered 1 as the first integration point at the bottom and in sequential order to the integration point at the top.

Sample:

no sample.

Dialog:

Interface

  • Shell to Solid : Map results from shell parts to solid parts.

  • Solid to Shell : Map results from solid parts to shell parts.

  • Shell to Shell : Map results from shell parts to shell parts.

  • Solid to Shell : Map results from solid parts to shell parts.

  • Target IPs : Specify through-thickness integration point numbers to map the results to. Only applicable to Solid to Shell mapping. *ELEMENT_SHELL_COMPOSITE will be created when this option is used.

  • From Parts : Activate to select the parts which have *INITIAL_STRESS data.

  • To Parts : Activate to select the parts which you want to map the *INITIAL_STRESS data to.

  • Fully Integrated : Activate this option to create *INITIAL_STRESS with 4 in-plane integration points for shell elements and 8 integration points for solid elements.

  • Side 1 : Specify one topological side (top/bottom) of the solid.

  • Side 2 : Specify the other topological side (top/bottom) of the solid.

  • *INITIAL_STRESS : Activate to map stress values.

  • Plastic Strain : Activate to map plastic strain.

  • Thickness : Activate to map shell thickness.

  • History Variables : Activate to map history variables.

  • The "From - To"-table : This let the user specify which history variable number should be mapped and to which history variable number in the target parts. That is, you can for instance map history variable #5 to history variable #7 by enter From=5, To=7. May be useful when switching material model or element type.

  • Map : Perform the map operation.

  • Done : Exit result mapping interface.