# <!-- document.writeln("<font color=" + '#000000' + ">Plane Stress Bracket</font>"); //-->

## <!-- document.writeln("<font color=" + color4[0] + ">Introduction</font>"); //-->

This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS. The plane stress bracket tutorial builds upon techniques covered in the first tutorial (3D Bicycle Space Frame), it is therefore essential that you have completed that tutorial prior to beginning this one.

The 2D Plane Stress Bracket will introduce boolean operations, plane stress, and uniform pressure loading.

### <!-- document.writeln("<font color=" + color3[0] + ">Problem Description</font>"); //-->

The problem to be modeled in this example is a simple bracket shown in the following figure. This bracket is to be built from a 20 mm thick steel plate. A figure of the plate is shown below.

This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right.

## ANSYS Command Listing

```! Command File mode of 2D Plane Stress Bracket

/title, 2D Plane Stress Bracket

/prep7               ! Enter the pre-processor

! Create Geometry

BLC4,0,0,80,100
CYL4,80,50,50
CYL4,0,20,20
CYL4,0,80,20
BLC4,-20,20,20,60

CYL4,80,50,30		! Create Bolt Holes
CYL4,0,20,10
CYL4,0,80,10

ASBA,6,ALL		! Boolean Subtraction - subtracts all areas (other than 6) from base area 6

! Define Element Type

ET,1,PLANE82
KEYOPT,1,3,3		! Plane stress element with thickness

! Define Real Constants

! (Note: the inside diameter must be positive)
R,1,20	 ! r,real set number, plate thickness

! Define Material Properties

MP,EX,1,200000        ! mp,Young's modulus,material number,value
MP,PRXY,1,0.3         ! mp,Poisson's ratio,material number,value

! Define the number of elements each line is to be divided into
AESIZE,ALL,5    	  ! lesize,all areas,size of element

! Area Meshing
AMESH,ALL	  		! amesh, all areas

FINISH              ! Finish pre-processing

/SOLU               ! Enter the solution processor

ANTYPE,0			! Analysis type,static

! Define Displacement Constraints on Lines   (dl command)

DL, 7, ,ALL,0		! There is probably a way to do these all at once...
DL, 8, ,ALL,0
DL, 9, ,ALL,0
DL,10, ,ALL,0
DL,11, ,ALL,0
DL,12, ,ALL,0
DL,13, ,ALL,0
DL,14, ,ALL,0

! Define Forces on Keypoints  (fk command)

FK,9,FY,-1000		!fk,keypoint,direction,force

SOLVE                ! Solve the problem

FINISH               ! Finish the solution processor

SAVE                 ! Save your work to the database

/post1               ! Enter the general post processor

/WIND,ALL,OFF
/WIND,1,LTOP
/WIND,2,RTOP
/WIND,3,LBOT
/WIND,4,RBOT
GPLOT

/GCMD,1, PLDISP,2		! Plot the deformed and undeformed edge
/GCMD,2, PLNSOL,U,SUM,0,1	! Plot the deflection USUM

/GCMD,3, PLNSOL,S,EQV,0,1	! Plot the equivalent stress
/GCMD,4, PLNSOL,EPTO,EQV,0,1	! Plot the equivalent strain

/CONT,2,10,0,,0.0036		! Set contour ranges
/CONT,3,10,0,,8
/CONT,4,10,0,,0.05e-3

/FOC,ALL,-0.340000,,,1		! Focus point

/replot

PRNSOL,DOF,			! Prints the nodal solutions
```