14.3. Defining Reinforcing Sections and Elements

Creating reinforcing elements is a two-part process:

  1. 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:

  2. Generate the reinforcing elements to embed in other structural (base) elements.

14.3.1. Mesh-Independent Method

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 TypeMESH200 OptionsCompatible Base Elements [1]
Smeared (2-D)

2-D lines with 2 or 3 nodes

KEYOPT(1) = 0, 1

PLANE182, PLANE183

SHELL208, SHELL209

Smeared (3-D)

3-D surface with 3-node triangle or 4-node quadrilateral

KEYOPT(1) = 4, 6

SOLID185, SOLID285, SOLSH190, SHELL181

Discrete (3-D)

3-D lines with 2 or 3 nodes

KEYOPT(1) = 2, 3

SOLID185, SOLID186, SOLID187, SOLID285, SOLSH190,

SHELL181, SHELL281,

BEAM188, BEAM189,

PIPE288, PIPE289,

LINK180


  1. High-order 3-D solid (SOLID186 and SOLID187) and shell (SHELL281) elements are not supported for embedding 3-D smeared reinforcing.

Using the Mesh-Independent Method:

  1. Create the base elements.

  2. Create MESH200 elements with appropriate reinforcing (REINFnnn) sections.

  3. Select the base elements and the MESH200 elements.

  4. Generate the reinforcing elements (EREINF).

  5. Inspect and verify the newly created reinforcing elements.

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 (Main Menu> Preprocessor> Sections> Reinforcing> Display Options).

14.3.1.1. Example: Discrete Reinforcing (Mesh-Independent Method)

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:

Figure 14.3:  Discrete Reinforcing Element Display (with Translucent Base Elements)

Discrete Reinforcing Element Display (with Translucent Base Elements)

14.3.1.2. Example: 2-D Smeared Reinforcing (Mesh-Independent Method)

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:

Figure 14.4:  2-D Smeared Reinforcing Element Display (with Translucent Base Elements)

2-D Smeared Reinforcing Element Display (with Translucent Base Elements)

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.

14.3.1.3. Example: 3-D Smeared Reinforcing (Mesh-Independent Method)

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:

Figure 14.5:  3-D Smeared Reinforcing Element Display (with Translucent Base Elements)

3-D Smeared Reinforcing Element Display (with Translucent Base Elements)

Figure 14.6:  Fiber Orientation Display on Smeared 3-D Reinforcing Elements

Fiber Orientation Display on Smeared 3-D Reinforcing Elements

14.3.2. Standard Method

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:

  1. Create the base elements.

  2. Build the reinforcing sections, with locations defined with respect to base elements via standard location patterns.

  3. Select the base elements elements to reinforce.

  4. Generate the reinforcing elements (EREINF).

  5. 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 (Main Menu> Preprocessor> Sections> Reinforcing> Display Options).

14.3.2.1. Example: Discrete Reinforcing (Standard Method)

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:

Figure 14.7:  Discrete Reinforcing Element Display (with Translucent Base Elements)

Discrete Reinforcing Element Display (with Translucent Base Elements)

14.3.2.2. Example: Smeared Reinforcing (Standard Method)

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:

Figure 14.8:  Smeared Reinforcing Element Display (with Translucent Base Elements)

Smeared Reinforcing Element Display (with Translucent Base Elements)

Figure 14.9:  Fiber Orientation Display on Smeared Reinforcing Elements

Fiber Orientation Display on Smeared Reinforcing Elements

14.3.3. Generating Reinforcing Elements

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:

14.3.3.1. Using EREINF with the Mesh-Independent Method

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 LocationEREINF Action
Fully embedded in a homogeneous solid element Accept
Fully outside of a homogeneous solid elementReject
Partially embedded in a homogeneous solid elementKeep only the portion embedded
Non-parallel to a link, beam, or pipe elementReject
Outside of the cross-section of a link, beam, or pipe elementReject
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 elementReject
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

14.3.3.2. Using EREINF with the Standard Method

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.


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