EREINF

EREINF, KOffALim, KTri
Generates reinforcing elements from selected existing (base) elements.

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

KOffALim

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.
KTri

Specify the shape of 3D smeared reinforcing members. Valid for the mesh-independent method only.

0 – Generate quad-dominant (mixed quadrilateral and triangular) reinforcing members (default).
1 – Generate triangular reinforcing members only.

Notes

EREINF 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 EREINF, 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.

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

Elements generated by EREINF are not associated with the solid model.

After EREINF executes, you can issue ETLIST, ELIST, or EPLOT 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 EREINF only after the base elements are finalized. If you delete or modify base elements (via EDELE, EMODIF, ETCHG, EMID, EORIENT, NUMMRG, or NUMCMP, for example), remove all affected reinforcing elements and reissue EREINF to avoid inconsistencies.

If you define reinforcing via the mesh-independent method, EREINF creates new reinforcing sections containing details of the created reinforcing elements, then applies them to all newly generated reinforcing elements. The number of new reinforcing sections depends on the number of new reinforcing elements. (You can examine the properties of new sections (SLIST).) The program sets the ID number of the newest reinforcing section to the highest section ID number in the model. After issuing EREINF, the command shows the highest-numbered IDs (element type, element, and section). Do not overwrite a new reinforcing section when defining subsequent sections.

For the 3D smeared-reinforcing element (REINF265) with the mesh-independent method, you can select the shape of the reinforcing members via KTri. The default behavior (KTri = 0) generates quad-dominant members (primarily quadrilaterals but with some triangles).

EREINF can generate the reinforcing elements with thermal properties if the base elements are thermal solid elements (SOLID278 or SOLID279):

  • If using the mesh-independent method for defining reinforcing, apply element body-force loading (BFE,,HGEN) or nodal body-force loading (BF,,HGEN) on the MESH200 elements.

  • If using the standard method for defining reinforcing, apply element body-force loading (BFE,,HGEN) on the reinforcing members directly. (Do not apply nodal body-force loading (BF,,HGEN).)

If performing a subsequent structural analysis after the thermal analysis, EREINF can convert the reinforcing elements for the structural analysis:

  1. Convert the thermal base elements to the appropriate structural element (ET or EMODIF).

  2. Select the reinforcing elements only.

  3. Issue EREINF.

    Result: The selected reinforcing elements are converted to elements compatible with the converted base elements.

Solution accuracy can be affected if the volume ratio between reinforcing elements and base elements is high (this condition is referred to as “base mesh overloading”), particularly when body loading (such as heat generation) is applied via the reinforcing elements. If the program detects a high volume ratio of reinforcing elements generated via the mesh-independent method, it issues a warning message and saves affected base and MESH200 elements (used to generate the reinforcing elements) into a component for close model inspection. Only the volume of reinforcing elements created by the current EREINF command is considered in the volume-ratio calculation (that is, no volume accumulation occurs over multiple EREINF commands).

To overcome solution accuracy issues due to base mesh overloading, the base mesh can be optimized according to the reinforcing requirements via the MSHOPTIM command. For more details about the requirements and limitations, refer to the MSHOPTIM command.

For more information, see Reinforcing and Direct Element Embedding in the Structural Analysis Guide.

Menu Paths

This command cannot be accessed from a menu.