Generates reinforcing elements from selected existing (base) elements.

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –


Enable or disable the limit of the angle between a MESH200 element and a base element. Valid for the mesh-independent method only.

0 – Enable the angle limit (default).
1 – Disable the angle limit.


The EREINF command generates reinforcing elements (REINF263, REINF264 and REINF265) directly from selected base elements (that is, existing standard structural elements in your model). The command scans all selected base elements and generates (if necessary) a compatible reinforcing element type for each base element. (You can select a combination of different base element types.)

Before issuing the EREINF command, first define the reinforcing geometry, material, and orientation via one of two methods:

Mesh-Independent Method:  Use MESH200 elements to temporarily represent the geometry of the reinforcing fibers or smeared reinforcing surfaces. Define additional data including material, fiber cross-section area, fiber spacing, and fiber orientation via reinforcing sections with the mesh pattern (SECDATA) and assign the sections to corresponding MESH200 elements. (Predefining the reinforcing element type [ET] is not required.)

Standard Method:  Define reinforcing section types (SECTYPE) with standard reinforcing location patterns (SECDATA). The standard reinforcing location input are given with respect to the selected base elements; therefore, a change in the base mesh may require redefining the (mesh-dependent) reinforcing section types.

Standard element-definition commands (such as ET and E) are not used for defining reinforcing elements.

The EREINF command creates no new nodes. The reinforcing elements and the base elements share the common nodes.

Elements generated by this command are not associated with the solid model.

After the EREINF command executes, you can issue ETLIST, ELIST, and EPLOT commands to verify the newly created reinforcing element types and elements.

Reinforcing elements do not account for any subsequent modifications made to the base elements. ANSYS, Inc. recommends issuing the EREINF command only after the base elements are finalized. If you delete or modify base elements (via EDELE, EMODIF, ETCHG, EMID, EORIENT, NUMMRG, or NUMCMP commands, for example), remove all affected reinforcing elements and reissue the EREINF command to avoid inconsistencies.

If you define reinforcing via the mesh-independent method, the EREINF command also integrates all reinforcing sections referenced by MESH200 elements and creates a single new reinforcing section, applying it to all newly created reinforcing elements. You can examine the properties of the new section (SLIST). The program sets the section ID number for the new reinforcing section to the highest section ID number in the model. Do not overwrite the new reinforcing section when defining subsequent sections.

For more information, see Reinforcing in the Mechanical APDL Structural Analysis Guide.

Menu Paths

This command cannot be accessed from a menu.

Release 18.2 - © ANSYS, Inc. All rights reserved.