8

Built-Up Beams

Modal Analysis

Determine the first two natural frequencies of the micro-electromechanical system (MEMS) cantilever beam shown here using the built-up beam feature. The beam cross-section is made of three layers of aluminum embedded in silicon and the beam length is 100 m. All dimensions and properties are in MKSV units.

Brief Instructions

  1. Start ANSYS 5.7 with the default jobname (file).
  2. Create a rectangle that is 2 m acrossand 3.5 m in height and symmetrical about the origin.
  3. Set the element edge length on all lines to be 0.5 m.
  4. Write the area as a custom section to a file, name the file “beam.SECT”.
  5. Clear the database.
  6. Edit the custom section by modifying the aluminum elements to reference material number 2.
  7. Input the file “beam.inp”.
  8. Read in the section mesh “built-up.SECT” as section ID number 1.
  9. Do an element plot to see the resulting beam cross-section mesh.
  10. Solve the modal analysis.
  11. List the Results Summary.
  12. Exit ANSYS.

Detailed Instructions

  1. Start ANSYS 5.7 with the default jobname (file).
  2. Create a rectangle that is 2 m across and 3.5 m in height and symmetrical about the origin.

Click on:

Main Menu > Preprocessor > -Modeling- Create > -Areas- Rectangle > By Dimensions

X1 = -1

X2 = 1

Y1 = -1.75

Y2 = 1.75

[OK]

Or issue:

/PREP7

RECTNG,-1.0,1.0,-1.75,1.75

  1. Set the element edge length on all lines to be 0.5 m.

Click on:

Main Menu > Preprocessor > Size Cntrls > -Lines- All Lines

SIZE = 0.5

[OK]

Or issue:

LESIZE,ALL,0.5

  1. Write the area as a custom section to a file, name the file “beam.SECT”.

Click on:

Main Menu > Preprocessor > Sections > -Beam- Custom Sectns > Write from Areas

Read the Note that comes up, then click [Close]

In the “Select areas” window, click [Pick All]

FILE = beam.SECT

[OK]

  1. Clear the database.

Click on:

Utility Menu > File > Clear & Start New

[OK]

Answer [Yes] to the verification question

Or issue:

FINISH

/CLEAR

  1. Edit the custom section by modifying the aluminum elements to reference material number 2.

Click on:

Main Menu > Preprocessor > Sections > -Beam- Custom Sectns > Edit/Built-up

Select [Edit Custom]

FILE = beam.SECT

[OK]

Select [Modify Material]

Pick the aluminum elements (shown below)

[OK]

MAT = 2

[OK]


Select [Save]

FILE = built-up.SECT

[OK]

Select [Finish]

  1. Input the file “beam.inp”.

Click on:

Utility Menu > File > Read Input From

beam.inp

[OK]

Or issue:

/INPUT,beam,inp

NOTE: This input file creates the cantilever beam model using BEAM188 elements, defines the material properties, and specifies the modal analysis solution options.

  1. Read in the section mesh “built-up.SECT” as section ID number 1.

Click on:

Main Menu > Preprocessor > Sections > -Beam- Custom Sectns > Read Sect Mesh

Section ID number = 1

Section Name = built-up

FILE = [built-up.SECT]

[OK]

Or issue:

SECTYPE,1,BEAM,MESH,built-up

SECOFFSET,CENT

SECREAD,built-up,SECT,,MESH

  1. Do an element plot to see the resulting beam cross-section mesh.

Click on:

Utility Menu > Plot > Elements

Or issue:

EPLOT

  1. Solve the modal analysis.

Click on:

Main Menu > Solution > -Solve- Current LS

[OK]

Or issue:

/SOLUTION

SOLVE

  1. List the Results Summary.

Click on:

Main Menu > General Postproc > Results Summary

Or issue:

/POST1


SET,LIST

  1. Exit ANSYS.

Click on:

Main Menu > File > Exit

Choose Quit – No Save!

[OK]

Or issue:

FINISH

/EXIT,NOSAVE

ANSYS 5.7 New Features Workshop Supplement8-1