V A B S Variable Asymptotic Beam Section

1
V A B SVariable Asymptotic Beam Section
Introduction and tutorial for VABS-ANSYS toolkit
M. Emre Gündüz Integrated Product Life-cycle
Engineering Laboratory ( I P L E ) Georgia
Institute of TechnologyOctober 2006
Some portions of this presentation are taken from
documentation that comes with VABS
2
What is VABS

• VABS (Variable Asymptotic Beam Section) is a
  computer program that implements a variable
  asymptotic method for computing the stiffness of
  a heterogeneous beam at a given cross section.
• VABS is based on the variational-asymptotic
  method, a rigorous mathematical technique by
  which a 3-D representation of a thin elastic body
  (such as a beam or plate) can be methodically
  reduced to a 1-D or 2-D model.
• Used in calculating rotor blade stiffnesses

3
Place in analysis

• For structural and dynamic analysis of the
  rotor/blade

Dynamic properties
CATIA
ANSYS
VABS
DYMORE
Stiffnesses
Crossectional Geometry
2-D Mesh
Material properties
Geometrical features
4
How it works

• It is a single executable DOS file

input
output
VABS.exe
file.dat (ASCII text file)
file.dat.K (ASCII text file)
5
What goes in

• Input file contains information about the
  geometry of the meshed crossection.
• It has coordinates of each node,
• all the nodes forming each element,
• material properties,
• etc.

6
Input file
F the flag for input file of old vabs F
F T F F F 13 2 1
nnode, nelem, nmate 1 -0.500000
-1.000000 coordinates according to each
node 2 0.500000 -1.000000 3
0.000000 -1.000000 4 0.500000
1.000000 5 0.500000 -0.500000 6
0.500000 0.000000 7 0.500000
0.500000 8 -0.500000 1.000000 9
0.000000 1.000000 10 -0.500000
0.500000 11 -0.500000 0.000000 12
-0.500000 -0.500000 13 0.000000
0.000000 1 1 2 6 11 3 5
13 12 0 nodes forming each
elelment 2 11 6 4 8 13 7
9 10 0 1 1 0 0.000000 540.00 0.00
0.00 0.00 0.00 0.00 0.00
0.00 2 1 0 0.000000 540.00 0.00 0.00
0.00 0.00 0.00 0.00 0.00 0.26E10
0.26E10 0.26E10 E1 E2 E3 0.1E10 0.1E10
0.1E10 G12 G13 G23 .300000000E00
.300000000E00 .300000000E00 U12 U13 U23
(Poisson's ratios) 1000 rho
7
VABS-ANSYS toolkit

• Generates the input file using mesh tool in ANSYS
• In form of ANSYS macros
• Requires an unmeshed 2-D geometry and material
  properties

8
Tutorial

• We will get properties of a rectangular beam
  crossection made of two different isotropic
  materials steel and aluminium
• tutorial.mtl file has the material properties
• For isotropic materials E1E2E3
  and G12G13G23 E / 2(1?)

9
Step by step tutorial (1)

• Open ANSYS
• The geometry MUST be inYZ plane Workplane
  offset WP by increments
• Bring the slider to 90 degrees
• Click X once, then Y once - OK
• Preprocessor modeling- create areas -
  rectangle by 2 corners
• WP X-0.5 WP Y-0.5 Width1 Height0.5
  OK

10
Step by step tutorial (2)

• Click Right view button on the right.
• Preprocessor modeling- create areas -
  rectangle by 2 corners
• WP X-0.5 WP Y0 Width1 Height0.5 OK
• PlotCtrls Numbering...
• Check AREA and LINE numbers
• Write down the area numbers for each area. Here
  we will use steel for the area on the left, and
  aluminium for the area on the right

11
Step by step tutorial (3)

• Make sure area numbering starts from 1 and ends
  at 2. The numbers of areas must be in order for
  the macro to work.
• Also, adjacent areas must share the same line
  between them. Make sure there are no lines on top
  of each other. We have such a situation in this
  case Line 3 and Line 5. The remedy to this
  problem is gluing the areas together
• Preprocessor Modeling Operate Booleans
  Glue - Areas

12
Step by step tutorial (4)

• Select A1 and A2 with left click. Make sure Count
  2 as in the figure on the right OK
• Now A2 is skipped. We have A1 and A3. To fix
  this, go to Preprocessor NumberingCtrls
  Compress Numbers
• Select All in the menu OK
• If nothing changes, go to Plot Replot
• Now there must be two areas A1 and A2 and seven
  lines. To check this, go to List Lines

13
Step by step tutorial (5)

• Click OK

• There must be total of seven lines. Now close
  this window
• Make sure .mac files and material file
  (tutorial.mtl) is in working directory. If not,
  copy everything in C\VABS 2.1.1\VABS-ANSYSmacroVe
  r2test into C\Documents and Settings\guest\

14
Step by step tutorial (6)

• Enter in the command line vabsinp
• This initiates the macro sequence. It will ask
  you a number of questions. The square bracketed
  numbers are default values
• Enter file name tutorial (must be same as .mtl
  file)
• Number of materials 2
• Material for Area 1 1 (aluminium)
• Material is isotropic 0
• Enter 1 to accept your input

15
Step by step tutorial (7)

• Material for Area 2 2 (steel)
• Material is isotropic 0
• Enter 1 to accept your input
• It should now mesh the model.

Check the output window. It should say COMPLETE
somewhere close to the bottom.
16
Step by step tutorial (8)

• We are done with ANSYS (BUT DO NOT CLOSE IT YET)
• (optionally) You may open tutorial.dat in Notepad
  to view the file.
• Now run VABS.exe
• Enter tutorial.dat
• It will generate a tutorial.dat.K file

17
Anisotropic materials (1)
I. Sign convention of layups  To understand VABS
layup, we need to find relationship between three
coordinate systems, the global system (x_i) used
by the user to define the geometry, the material
system (e_i) used by the user to define the
material properties, and an aided one to define
the ply plane (y_i). The ply plane can be
described using y1 and y2, where y1 is parallel
to x1, It is assumed that the ply plane is
rotating in the plane of cross section stretched
by y2 and y3 axes (see figure). Then the rotation
angle between y2 and x2 is named as ?1. y3 is
determined by y1 and y2 to form a right hand
system. We set the value range of ?1 to 0, 360
degrees).
Figure. The orientation of ply plane (y1, y2, y3)
in global reference system (x1, x2, x3)
18
Anisotropic materials (2)
In figure below , the relation between ply plane
(Y1, Y2, Y3) and material system (e1, e2, e3) is
shown. Let the material normal axis e3 be the
same as the ply plane normal Y3, and the rotation
between e1 ( fiber direction ) and Y1 be ?3
which is usually called layup orientation in
engineering applications. We set the value range
of ?3 between (-90,90.
Figure. The orientation of material system (1, 2,
3) in ply plane system (Y1, Y2, Y3)
19
Anisotropic materials (3)

• For curved surfaces
• Laminate orientation angle (ß ?1 previously) is
  defined by a mold contour in manufacturing
• It is automatically calculated for each element
  using a manually picked reference edge

Laminate Orientation in a Cross Section
20
Anisotropic materials (4)

• This Reference Edge must be an edge of the area
  that is parallel to the edge of the lamina in the
  cross section.
• When asked, pick the line with the normal vector
  pointing away from the area as the reference
  edge.

• Ply lay-up orientation angle (a?3 of previous
  slide) is manually entered in ANSYS

21
Step by step tutorial (9)

• We will now substitute steel with an anisotropic
  material Generic S-glass/Epoxy Unidirectional
  Prepreg
• Enter the following instead of steel properties
  in tutorial.mtl and save it.

• 43000E6 8900E6 8900E6
• 4500E6 4500E6 4500E6
• 0.27 0.27 0.27
• 2000

22
Step by step tutorial (10)

• In ANSYS go to Preprocessor Meshing Clear
  Areas
• Click Pick All
• Then go to Plot Areas
• Run vabsinp and repeat everything in tutorial (6)
• For the second area, the material is anisotropic,
  so enter anything other than 0, say, 5

23
Step by step tutorial (11)

• Select one of the long lines on the sides of the
  area. Click OK
• Enter 45 as layup angle

• Complete the meshing process as done before
  tutorial (7). Obtain the .dat.K file using VABS
  tutorial (8).

24
Results (1)

VARIATIONAL ASYMPTOTIC BEAM SECTIONAL
ANALYSIS
SCHOOL OF
AEROSPACE ENGINEERING
GEORGIA INSTITUTE OF TECHNOLOGY

THE 6X6 MASS MATRIX (ACCORDING TO
DYMORE CONVENTION)
0.271139D01
0.000000D00 0.000000D00
0.000000D00 0.175336D-17
-0.429361D-17 0.000000D00
0.271139D01 0.000000D00
-0.175336D-17 0.000000D00
0.000000D00 0.000000D00
0.000000D00 0.271139D01
0.429361D-17 0.000000D00
0.000000D00 0.000000D00
-0.175336D-17 0.429361D-17
0.143658D-02 0.000000D00
0.000000D00 0.175336D-17
0.000000D00 0.000000D00
0.000000D00 0.700683D-03
0.166760D-20 -0.429361D-17
0.000000D00 0.000000D00
0.000000D00 0.166760D-20
0.735894D-03 THE MASS CENTER

Xm2 1.583545054957183E-018 Xm3
6.466636937781354E-019 THE CENTROID OF THE
CROSS SECTION (PURELY GEOMETRIC)

X2 -2.495522444475189E-019 X3
-1.677308361824522E-018 STIFFNESS - WITHOUT
CORRECTION
1-extension 2-twist 3- and
4-bending 0.24570392E08
0.00000000E00 -0.26914267E01
-0.10933518E02 0.00000000E00
0.63131533E03 0.00000000E00
0.00000000E00 -0.26914267E01
0.00000000E00 0.12282367E05
0.99993090E-01 -0.10933518E02
0.00000000E00 0.99993090E-01
0.12786287E05
Mass per unit span
Moments of inertia
25
Results (2)
THE NEUTRAL AXES
Xe2 4.449875441282011E-
007 Xe3 -1.095394294096603E-007
TIMOSHENKO STIFFNESS MATRIX
1-EXTENSION
2,3-SHEAR 4-TORSION 5,6-BENDING
0.24570392E08 0.00000000E00
0.00000000E00 0.00000000E00
-0.26914267E01 -0.10933518E02
0.00000000E00 0.17275858E07
-0.14034151E02 -0.39824686E00
0.00000000E00 0.00000000E00
0.00000000E00 -0.14034151E02
0.17089713E07 0.55218219E-01
0.00000000E00 0.00000000E00
0.00000000E00 -0.39824686E00
0.55218219E-01 0.63131534E03
0.00000000E00 0.00000000E00
-0.26914267E01 0.00000000E00
0.00000000E00 0.00000000E00
0.12282367E05 0.99993090E-01
-0.10933518E02 0.00000000E00
0.00000000E00 0.00000000E00
0.99993090E-01 0.12786287E05 THE SHEAR
CENTER OF THE CROSS SECTION
E2
3.230890126371592E-008 E3
2.305219325956943E-007
Shear stiffness
Bending stiffness
Torsional stiffness
Axial stiffness
26
Blade sections

• A bearingless rotor blade

• (Concept originally designed by Tom Hanson, CAD
  drawings performed in ITU)

27
Setting crossections
28
(No Transcript)
29
Import into ANSYS
30
Exercise (1)

• Get stiffnesses for the crossection below
• The file name is cr02.igs
• Material file is cr02.mtl. It has two materials.
  The first one is isotropic, the second one is
  composite

• Layup angle is 0, and reference edges are the
  longer sides of the four rectangular crossections

Material 2
Material 1
31
Exercise (2)

• Importing .igs files into ANSYS
• File import IGES...
• Click OK
• Click Browse to find the file to open - OK

32
Exercise (3)

• The geometry has no areas in it. You have to
  create them using the lines.
• Preprocessor Modeling Create Areas
  Arbitrary By Lines
• Click four lines of any rectangle then click
  apply. Repeat for the remaining three rectangles.
  
• The last area is the middle part. Click on all
  the lines enclosing the middle part. Then click
  OK
• It should look like the next slide...

33
(No Transcript)
34
Exercise (5)

• Follow the steps in the tutorial to get results
• When you are done, compare your cr02.dat file and
  cr02.dat.K file with provided files.
• They may not be identical, because element size
  was different in the macro for that analysis
• For more information, read the reference for this
  presentation UserManualV1.1.pdf
• You can ask me questions later in person or via
  e-mail
• Office ESM building room 306 or G-13
• E-mail emre_at_gatech.edu