Sign-up for free online course on ANSYS simulations!Unable to render {include} The included page could not be found.
Author: Ben Mullen, Cornell University
Problem Specification
1. Pre-Analysis & Start-Up
2. Geometry
3. Mesh
4. Setup (Physics)
5. Solution
6. Results
7. Verification & Validation
Setup (Physics)
Set Material Properties
Outer Surface
Because the thickness of the blade varies, we need to set the material via commands. First, we will create a command that governs the material properties of the outer surface of the blade. To create a command, right click on the Outer Surface surface body, and select Insert > Commands. In the command prompt, insert the following:
/prep7 !Call the Preprocessor
et,matid,181 !Specify the element type, shell 181
keyopt,matid,3,2 !Use full integration
mpdel,all,matid !Delete all previously assigned material properties
tbdel,all,matid !Delete all previouly assigned tabular data
MP,EX,1,33E9 !Define Young's Modulus: X Direction
MP,EY,1,33E9 !Define Young's Moduls: Y Direction
MP,EZ,1,33E9 !Define Young's Modulus: Z Direction
MP,PRXY,1,0.3 !Define Major Poisson's ratio XY
MP,PRYZ,1,0.3 !Define Major Poisson's ratio YZ
MP,PRXZ,1,0.3 !Define Majoy Poisson's ration XZ
Spar
Create a command for the spar, and insert the following
/prep7 !Call the Preprocessor
et,matid,181 !Specify the element type, shell 181
keyopt,matid,3,2 !Use full integration
mpdel,all,matid !Delete all previously assigned material properties
tbdel,all,matid !Delete all previouly assigned tabular data
MP,EX,2,101E9 !Define Young's Modulus: X Direction
MP,EY,2,101E9 !Define Young's Moduls: Y Direction
MP,EZ,2,101E9 !Define Young's Modulus: Z Direction
MP,PRXY,2,0.3 !Define Major Poisson's ratio XY
MP,PRYZ,2,0.3 !Define Major Poisson's ratio YZ
MP,PRXZ,2,0.3 !Define Major Poisson's ration XZ
Setup Varying Thickness function
Outer Surface
Now, we need to set up the varying thickness function governing the blade's thickness. To do this, we will need to open ANSYS APDL. To open, go to Start > All Programs > ANSYS 13.0 > Mechanical APDL (ANSYS). Once ANSYS APDL opens, go to Parameters > Functions > Define/Edit. The function that will drive the thickness is 0.030 - 0.00048485X where X is the distance from the origin along the X-axis. In the Result text box, type .03 - 0.00048485*, then, to input the x variable, open the drop down menu next that is defaulted to Time and change it to X.
Press ENTER. Then in the Function Editor window, go to File > Save. Change the Save as type to All Files, and name the file vth.txt. Once you save, you may close ANSYS APDL. Now, open the text file you just created. We need to name the function. In the text file, use Replace to replace all instances of %_FNCNAME% with vth. Also, we need to add the line
sect,1,shell !Specify the section type
secfunction,%vth% !Apply the Varying Thickness Function
to the end of the code. For simplicity, I have posted the entire code here:
*DIM,vth,TABLE,6,5,1, !Dimension The Table for the Thickness Function
! Begin of equation: .030-{X}*.00048485
!30mm at root and 10mm at tip
vth(0,0,1)= 0.0, -999
vth(2,0,1)= 0.0
vth(3,0,1)= 0.0
vth(4,0,1)= 0.0
vth(5,0,1)= 0.0
vth(6,0,1)= 0.0
vth(0,1,1)= 1.0, -1, 0, .00048485, 0, 0, 2
vth(0,2,1)= 0.0, -2, 0, 1, 2, 3, -1
vth(0,3,1)= 0, -1, 0, .030, 0, 0, -2
vth(0,4,1)= 0.0, -3, 0, 1, -1, 2, -2
vth(0,5,1)= 0.0, 99, 0, 1, -3, 0, 0
! End of equation: .030-{X}*.00048485
sect,1,shell !Specify the section type
secfunction,%vth% !Apply the Varying Thickness Function
Post this code at the end of the command snippit you created for the Outer Surface.
Spar
We need to repeat the above step, creating a command for the spar, but this time the thickness will be constant at 0.20 m. We will also have to make minute changes to the code to refer to the correct section. For simplicity, the code is posted below. Copy and paste the code below into the command snippit for the Spar.
*DIM,sth,TABLE,6,5,2, !Dimension The Table for the Thickness Function
! Begin of equation: .020
sth(0,0,1)= 0.0, -999
sth(2,0,1)= 0.0
sth(3,0,1)= 0.0
sth(4,0,1)= 0.0
sth(5,0,1)= 0.0
sth(6,0,1)= 0.0
sth(0,1,1)= 1.0, 99, 0, .10, 0, 0, 0
sth(0,2,1)= 0
sth(0,3,1)= 0
! End of equation: .020
!-->
sect,2,shell !Specify the section type
secfunction,%sth% !Apply the Varying Thickness Function
Prevent ANSYS from changing Material Properties
We need to create one more command in order to ensure that ANSYS uses the varying thickness. In the Outline window, right click Static Structural (B5) and select Insert > Commands. Copy and paste the code below into the command window
fini !Exit current Module
/prep7 !Call the preprocessor
etcon,off !Disable ANSYS from changin any KEYOPTS
fini !Exit the preprocessor
/solu !Call the Solve Module
Fixed Support
We will fix the ring at the end of the blade. To accomplish this, click on Static Structural (B5) to bring up the Environment menu bar. In the Environment menu bar, select Supports > Fixed Support. Next, make sure the edge selection filter 
is selected. Hold Ctrl, and click on the 2 edges that make up the ring at the end shoulder of the blade (see image below).
When both edges have been selected, press Geometry > Apply.
Force Load
We want to apply a 1000 N downward force on the blade. To initialize a force load, in the Environment menu bar select Loads > Force. Make sure the surface selection filter 
is selected and choose the upper surface of the end of blade, as shown in the image below.
When the surface have been selected, press Geometry > Apply in the Details window. Next, select Define By > Components. Define the Y Component as -1000 N.
We are now ready to set up the solution and solve.