Creating reinforcing elements is a two-part process:
Define the reinforcing material, geometry (such as fiber location, cross-section area, and fiber spacing), and fiber orientation.
Two methods are available for defining reinforcing:
Generate the reinforcing elements to embed in other structural (base) elements.
The mesh-independent method offers much flexibility when the base elements are arbitrary and have no distinct patterns for the reinforcing to attach.
The reinforcing location is represented via a mesh with
MESH200 elements. Other model information, including
reinforcing material, cross-section area, spacing, and orientation, can be provided
via by a reinforcing element (REINFnnn) section
(SECDATA) or MESH200 element data.
MESH200 elements can be combined with base elements and reinforcing sections in various ways:
Table 14.1: MESH200 Element Options
| Reinforcing Type | MESH200 Options | Compatible Base Elements [1] |
|---|---|---|
| Smeared (2-D) |
2-D lines with 2 or 3 nodes KEYOPT(1) = 0, 1 | |
| Smeared (3-D) |
3-D surface with 3-node triangle or 4-node quadrilateral KEYOPT(1) = 4, 6 | |
| Discrete (3-D) |
3-D lines with 2 or 3 nodes KEYOPT(1) = 2, 3 |
Using the Mesh-Independent Method:
As shown in the following example input listings, you can manually adjust the translucency of the base elements to show the reinforcing elements. Additional automatic reinforcing display options are available via the GUI ().
Following is a typical sequence of commands for defining discrete reinforcing elements:
/batch,list /show,sample,grph /title, Example input data for generating discrete reinforcing elements /prep7 ! ! define material properties ! mp, ex,1,10e6 ! Base Material mp, ex,2,30e6 ! Reinforcing Material mp,prxy,1,.3 mp,prxy,2,.3 mp,dens,1,.00001 mp,dens,2,.00002 ! define base elements et,1,SOLID285 mat,1 block,0,10,0,1,0,2 esize,2 vmesh,1 ! ! Define discrete reinforcing section ! sectype,2,reinf,discrete secdata,1,0.1, MESH ! only MESH pattern is allowed for MESH200 ! ! Define MESH200 elements ! et,2,200,2 mat,2 secnum,2 numstr,line,1001 k,1001,-0.1, 0.5, 1.0 k,2001,10.1, 0.5, 1.0 l,1001,2001 lesize,1001,,,1 lmesh,1001 ! ! Create reinforcing elements via EREINF command ! esel,all EREINF ! ! Inspect newly created reinforcing elements ! esel,s,type,,1 ! adjust the translucency level of the ! base element to reveal the embedded reinforcing ! elements /trlcy,elem,0.9 esel,all /view,1,1,1,1 ! Activate the expanded element shapes /eshape,1 eplot
The input listing generates the following output:
Following is a typical sequence of commands for defining 2-D smeared reinforcing elements:
/batch,list /show,sample,grph /title, Example input data for generating 2D smeared reinforcing elements /prep7 ! ! define material properties ! mp, ex,1,10e6 ! Base Material mp, ex,2,30e6 ! Reinforcing Material mp,prxy,1,.3 mp,prxy,2,.3 mp,dens,1,.00001 mp,dens,2,.00002 ! define base elements et,1,183 rect,0,10,0,2 esize,2 amesh,1 ! ! Define discrete reinforcing section ! sectype,2,reinf,smea secdata,1,0.1,0.01,,,MESH !Only MESH pattern allowed for MESH200 ! ! Define MESH200 elements ! et,2,200,0 k,10,-0.2,-0.2 k,11,10.5,2.5 l,10,11 type,2 secnum,2 esize,,1 lmesh,5 ! ! Create reinforcing elements via EREINF command ! esel,all EREINF ! ! Inspect newly created reinforcing elements ! esel,s,type,,1 ! adjust the translucency level of the ! base element to reveal the embedded reinforcing ! elements /trlcy,elem,0.9 esel,all ! Turn on the expaned element shapes /eshape,0.05 eplot fini
The input listing generates the following output:
A single new reinforcing section is created and applied to all newly created reinforcing elements. You can examine the properties of the new reinforcing section (SLIST). The program sets the section ID number of the new section to the highest section ID number in the model. When defining subsequent sections, avoid accidentally overwriting of the new reiniforcing section.
When reinforcing is embedded in the common face (or edge) of two or more neighboring base elements, the EREINF command suppresses duplicate reinforcing-to-base intersections. If the base mesh is non-conforming (that is, element faces/edges are partially overlapping), the EREINF command may suppress any 3-D smeared surface intersections that partially overlap with other intersections.
Following is a typical sequence of commands for defining 3-D smeared reinforcing elements:
/batch,list /show,sample,grph /title, Example input data for generating 3-D smeared reinforcing elements /prep7 ! ! Define material properties ! mp, ex,1,10e6 ! Base Material mp, ex,2,30e6 ! Reinforcing Material mp,prxy,1,.3 mp,prxy,2,.3 mp,dens,1,.00001 mp,dens,2,.00002 ! ! Define base elements ! et,1,SOLID285 block,0.0,10.0,0.0,1.0,0.0,2.0 mat,1 esize, 2.0 vmesh, 1 ! ! Define smeared reinforcing section ! sect,2,REINF,SMEAR secd,2,0.1,0.01,,45.0,MESH ! ! Define MESH200 elements ! et,2,200,6 type,2 secnum,2 mat,2 aoffst,3,-0.5 ASEL,,,,7 esize,1, local,11, esys,11 AMESH,all ! ! Create reinforcing element via EREINF ! esel,all csys,0 EREINF ! ! Inspect newly created reinforcing elements ! esel,s,type,,1 ! adjust the translucency level of the ! base element to reveal the embedded reinforcing ! elements /trlcy,elem,0.9 esel,all /view,1,1,1,1 eplot ! ! Verify the reinforcing fiber orientation ! ! Switch to the vector plot /dev,vect,1 ! Select only reinforcing elements (optional) esel,s,type,,3 /psymb,layr,-1 eplot finish
The input listing generates the following output:
All essential reinforcing data are defined via reinforcing element
(REINFnnn) sections. The reinforcing location is
given directly with respect to the base element connectivity. The standard method is
recommended only when the reinforcing location conforms to the base elements (such
as beams, pipes, and layered elements).
Using the Standard Method:
Create the base elements.
Build the reinforcing sections, with locations defined with respect to base elements via standard location patterns.
Select the base elements elements to reinforce.
Inspect and verify the newly created reinforcing elements.
As shown in Example: Discrete Reinforcing (Standard Method) and Example: Smeared Reinforcing (Standard Method), you can manually adjust the translucency of the base elements to show the reinforcing elements. Additional automatic reinforcing display options are available via the GUI ().
Following is a typical sequence of commands for defining discrete reinforcing elements via the standard method:
/batch,list /show, sample,grph /title, Example input data for generating discrete reinforcing elements /prep7 ! ! Define material properties ! mp, ex,1,10e6 ! Base Material mp, ex,2,30e6 ! Reinforcing Material mp,prxy,1,.3 mp,prxy,2,.3 mp,dens,1,.00001 mp,dens,2,.00002 ! ! Define base geometry ! k,1, 0.,0. k,2,10.,0. l,1,2 ! ! Define base elements ! et,1,BEAM188 mat,1 sect,1,BEAM,I secd,1.,1.,1.,0.2,0.2,0.3 esize, 2.0 lmesh, 1 ! ! Define discrete reinforcing section ! sect,2,REINF,DISC secd,2,0.01,BEAM,-0.25,0.1 secd,2,0.01,BEAM, 0 .0,0.1 secd,2,0.01,BEAM, 0.25,0.1 secd,2,0.01,BEAM,-0.25,0.9 secd,2,0.01,BEAM, 0 .0,0.9 secd,2,0.01,BEAM, 0.25,0.9 ! ! Create reinforcing element via EREINF ! esel,all secn, 2 ! use reinforcing section! EREINF ! ! Inspect newly created reinforcing elements ! esel,s,type,,1 ! adjust the translucency level of the ! base element to reveal the embedded reinforcing ! elements /trlcy,elem,0.9 esel,all /view,1,1,1,1 ! Turn on the expaned element shapes /eshape,1 eplot fini
The input listing generates the following output:
Following is a typical sequence of commands for defining smeared reinforcing elements via the standard method:
/batch,list /show, sample,grph /title, Example input data for generating smeared reinforcing elements /prep7 ! ! Define material properties ! mp, ex,1,10e6 ! Base Material mp, ex,2,30e6 ! Reinforcing Material mp,prxy,1,.3 mp,prxy,2,.3 mp,dens,1,.00001 mp,dens,2,.00002 ! ! Define base geometry ! CYLIND, 10.,12.,0.,20.,0,90. ! ! Define base elements ! et,1,SOLID185 mat,1 esize, 2.0 vmesh, 1 ! ! Define smeared reinforcing section ! sect,1,REINF,SMEAR secd,2,0.1,1.0,,45.0,ELEF,3,0.5 ! ! Create reinforcing element via EREINF ! esel,all EREINF ! ! Inspect newly created reinforcing elements ! esel,s,type,,1 ! adjust the translucency level of the ! base element to reveal the embedded reinforcing ! elements /trlcy,elem,0.9 esel,all /view,1,1,1,1 ! Turn on the expaned element shapes /eshape,1 eplot ! ! Verify the reinforcing fiber orientation ! ! Switch to the vector plot /dev,vect,1 ! Select only reinforcing elements (optional) esel,s,type,,2 /psymb,layr,-1 eplot fini
The input listing generates the following output:
A single EREINF command generates reinforcing elements according to your defined reinforcing material, geometry, and fiber orientation. The command determines the reinforcing element type, and creates and stores new reinforcing. (Standard element-definition commands such as ET and E are not used.)
Reinforcing elements ignore any subsequent modifications made to the base elements. ANSYS, Inc. recommends issuing the EREINF command only after you have finalized the base elements. If you delete or modify base elements after generating the reinforcing elements, remove all affected reinforcing elements and reissue the EREINF command to avoid inconsistencies.
The EREINF command operates differently according to the method used to define reinforcing:
The EREINF command determines the reinforcing element type according to the base element type, the MESH200 element type, and the reinforcing section associated with the MESH200 elements.
The command rejects MESH200 elements if their locations do not meet the requirements:
Table 14.2: Element Location and EREINF Command Action
| MESH200 Element Location | EREINF Action |
|---|---|
| Fully embedded in a homogeneous solid element | Accept |
| Fully outside of a homogeneous solid element | Reject |
| Partially embedded in a homogeneous solid element | Keep only the portion embedded |
| Non-parallel to a link, beam, or pipe element | Reject |
| Outside of the cross-section of a link, beam, or pipe element | Reject |
| Partially embedded in a link, beam, or pipe element | Keep only the portion embedded |
| Non-parallel to the shell surface or layers in a layered solid element | Reject |
| Outside of the shell section or the layered solid element | Reject |
| Partially embedded in a shell or layered solid element | Keep only the portion embedded |
The EREINF command determines the reinforcing element type according to the base element type and the current reinforcing section. The command generates no new reinforcing elements if the current section is not a valid reinforcing section or if the section is incompatible with the base elements.
To define a section ID to associate with subsequently-defined reinforcing elements, issue the SECNUM command.
Reinforcing locations are given with respect to the base element. Unexpected reinforcing placement may result from incorrectly oriented base elements. You can adjust the desired base element orientation (EORIENT or VEORIENT). In some cases, you may need to create different reinforcing sections for different base elements with inconsistent orientations.