WORKSHOP 4 LINEAR TRANSIENT ANALYSIS OF A CANTILEVERED BOX BEAM

1 / 54

# WORKSHOP 4 LINEAR TRANSIENT ANALYSIS OF A CANTILEVERED BOX BEAM - PowerPoint PPT Presentation

WORKSHOP 4 LINEAR TRANSIENT ANALYSIS OF A CANTILEVERED BOX BEAM. Problem Description: This model represents a hollow beam, which is fixed at one end; the overall beam dimensions are (h=40, w=20, l=600).

I am the owner, or an agent authorized to act on behalf of the owner, of the copyrighted work described.

## PowerPoint Slideshow about ' WORKSHOP 4 LINEAR TRANSIENT ANALYSIS OF A CANTILEVERED BOX BEAM' - nathan-serrano

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -
Presentation Transcript

WORKSHOP 4

LINEAR TRANSIENT ANALYSIS OF A CANTILEVERED BOX BEAM

Problem Description:

• This model represents a hollow beam, which is fixed at one end; the overall beam dimensions are (h=40, w=20, l=600).
• The model will be first analyzed using modal analysis techniques in order to determine the natural frequencies occurring in the cantilever. These results will then be compared to the theoretically predicted values for the beam.
• The results of this modal analysis will then be used to perform a modal dynamic analysis of the structure to find its response to a known sawtooth input. These results will then be compared to the results calculated for a linear-direct transient solution of the same system.

600

40

20

• Objective
• Extraction of modes for structure.
• Set-up and solution of modal transient problem.
• Set-up and solution of direct transient analysis.
• Comparison of solution techniques.
• Required
• No supporting file is required.

Suggested Exercise Steps:

• Extrude surfaces to form following beam (x=20; z=600); cap ends.
• Mesh beam using element size of 10 for perimeter and 20 for longitudinal axis.
• Define materials and shell properties.
• Set-up multiple load curves for analyses.
• Setup and solve modal analysis, comparison to theoretical.
• Setup small-displacements, modal frequency response analysis.
• Solve and monitor modal frequency analysis.
• Setup total-Lagrangian time-history dynamic analysis.
• Solve and monitor time-history dynamic analysis.
• Import and post-process results.
• Compare result techniques.
CREATE NEW DATABASE

a

cantilevered

c

b

cantilevered_beam

• Open a new database. Name itcantilevered_beam.db
• File: New
• Type cantilevered_beamas File name
• Click OK.
• Select MSC.Marc as the Analysis Code.
• Click OK.

d

MSC.Marc q

e

Step 1. Geometry: Create / Curve / PWL

a

b

[-10,-20,0],[10,-20,0],[10,20,0]

c

• Create curves by using PWL method.
• Geometry: Create / Curve / PWL.
• Enter [-10,-20, 0],[10,-20,0],[10,20,0],[-10,20,0],[-10,-20,0] as Point Coordinates List (A 20 by 40 rectangle).
• Click -Apply-.
Step 2. Geometry: Create / Surface / Extrude

a

b

<0, 0, 600>

e

c

Curve 1:4

f

d

• Create a surface by using Extrude method.
• Create / Surface / Extrude.
• Enter <0,0,600> as Translation Vector.
• Click into Curve List panel.
• Select Curve or Edge picking icon.
• Select Curve 1:4.
• Click –Apply-.
Step 3. Geometry: Create / Surface / Curve

c

a

b

Surface 3.2

e

Surface 1.2

h

f

• Create a surface by using Curve method.
• Create / Surface / Curve.
• Click into Starting Curve List panel.
• Select Curve or Edge picking icon.
• Select top end curve.
• Click into Ending Curve List panel.
• Choose Curve or Edge picking icon.
• Select bottom end curve.
• Click –Apply-.
• Repeat Steps b through h, then select the top and bottom rear curves (curve 3 and 1)to create Surface 6.

d

g

Step 4. Element: Create / Mesh Seed / Uniform

a

f

b

c

10

d

Curve 3 2

g

e

• Create mesh seed by using Uniform type.
• Elements: Create / Mesh Seed / Uniform.
• Select Element Length.
• Enter 10 as Length.
• Click Into Curve List panel.
• Select the Curve or Edge picking icon.
• Select the top and side curves of the beam.
• Click –Apply-.

k

h

20

i

Surface 2.3

l

j

• Enter 20 as Length.
• Click Into Curve List panel.
• Select the Curve or Edge picking icon.
• Select the longitudinal curves of the beam.
• Click -Apply-.
Step 5. Element: Create / Mesh / Surface

a

b

g

c

d

e

Surface 1:6

h

f

• Create / Mesh / Surface.
• Select Quad as Elem Shape.
• Select IsoMesh as Mesher.
• Click Into Surface List panel.
• Select the Curve or Edge picking icon.
• Select Surface 1:6.
• Click -Apply-.
Step 6. Elements: Equivalence / All / Tolerance

a

0.005

b

• Equivalence the nodes.
• Equivalence / All / Tolerance Cube.
• Click –Apply-.
Step 7. Materials: Create / Isotropic / Manual Input

a

d

30e6

e

0.3

f

7.45e-4

b

steel

g

c

h

• Giving the materials properties.
• Materials: Create / Isotropic / Manual Input.
• Enter steel as Material Name.
• Open Input Properties form.
• Enter 30e6 as Elastic Modulus.
• Enter 0.3 as Poisson Ratio.
• Enter 7.45e-4 as Density.
• Click OK.
• Click -Apply-.
Step 8. Properties: Create / 2D / Shell

a

b

shell

c

• Create properties.
• Properties: Create / 2D / Thin Shell.
• Enter shell as Property Set Name.
• Open Input Properties form.
• Enter Steel as Material Name.
• Enter 0.25 as Thickness.
• Close the form by clicking OK.

d

e

f

i

shell

g

Surface 1:6

j

h

k

• Click into the Select Members’ panel.
• Select the Surface or Face picking icon.
• Select Surface 1:6.
• Click -Apply-.
Step 9. Load/BCs: Create / Displacement / Nodal

a

d

<0, 0, 0>

e

<0, 0, 0>

i

Curve 1:4

j

b

wall

k

c

f

g

l

h

• Create a load boundary condition.
• Loads/BCs: Create / Displacement / Nodal.
• Enter wall as set name.
• Open Input Data form.
• Enter <0,0,0> as following translations vector.
• Enter <0,0,0> as following rotations vector.
• Click OK to close form.
• Open Select Application Region form.
• Select the Curve or Edge picking icon.
• select Curve 1:4.
• Click OK to close form.
• Click -Apply- to create displacement.
Step 10. Properties: Create

d

Displ_Wall

a

b

Fixed_End

c

f

e

• Create.
• Enter fixed_end as Load Case name.
• Select Displ_Wall.
• Click OK to implement changes.
• Click -Apply- to create load case.

Step 11. Analysis: Analyze / Entire Model / Full Run

d

modal

e

f

g

100

h

0

i

50

j

The selection of the upper bound for the extracted frequencies was based on initial predictions of the theoretical frequencies for the beam, as contained later in this document. If a good estimate of the required frequencies is not known, it is better to set the limit too high, than too low. It is also better to request a large number of modes for extraction, while controlling the number of extracted modes by the upper frequency bound.

• Analysis: Analyze / Entire Model / Full Run.
• Enter modal_job1 as Job Name
• Open Load Step Creation form.
• Enter modal as Job Step Name.
• Select Normal Modes as Solution Type.
• Open Solution Parameters form.
• Enter 100 as number of modes to extract.
• Enter 0 Hz for Lowest Frequency.
• Enter 50 Hz as Highest Frequency.
• Click OK to close form.

a

b

modal_job1

c

Defaultfixed_end

l

k

m

n

o

• Open Select Load Case form.
• Select fixed_end.
• Click OK to close form.
• Click -Apply- to finish step creation.
• Click Cancel to close form.

Default Static Stepmodal

q

r

Default Static Stepmodal

s

o

t

• Open Load Step Selection form.
• Click modal to add to analysis.
• Click Default Static Step to remove from analysis.
• Click OK to close form.
• Click on -Apply- to launch analysis.

modal_job1

Step 12. Analysis: Read Results / Result Entities / Attach

a

modal_job1

b

modal_job1

c

• Submit the result.
• Read Results / Result Entities / Attach.
• Select modal_job1.
• Click Apply.
Step 13. Results: Create / Quick Plot

a

b

c

d

e

• Open the Results form
• Results: Create / Quick Plot.
• Select Mode 1.
• Select Displacements, Translation for Fringe Result.
• Select Displacements, Translation for Deformation Result.
• Click on Deform attribute icon
• Change Scale Interpretation into Model Scale
• Set Scale Factor as 0.1
• Click -Apply- to display fringe plot.

e

e

f

Note that this is a bending mode about the weak axis, with a fundamental frequency of 2.753 Hz.

f

g

h

i

• Select Mode 2.
• Select Displacements, Translation for Fringe Result.
• Select Displacements, Translation for Deformation Result.
• Click -Apply- to display fringe plot.

Note that this is a bending mode about the strong axis, with a fundamental frequency of 4.616 Hz.

Mode 3 - A harmonic mode for bending about weak axis.

• Select Mode 3
• Select Displacements, Translation for Fringe Result.
• Select Displacements, Translation for Deformation Result.
• Click -Apply- to display fringe plot.
• Select Mode 33
• Click on Deform icon attribute
• Change Scale Interpretation into Model Scale
• Set Scale Factor as 0.02
• Click -Apply- to display fringe plot.

o

k

Mode 33 - A higher frequency mode for the side walls. From the sharpness displayed in the contours, the current mesh in inadequate to study these high frequency responses.

l

m

or

and

and

Where:

• Hand calculations
• Recalling from basic dynamics:
• For a cantilevered beam:
• For a beam in torsion:

Known information for beam:

Ix = 6518.12 in4

Iy = 2259.37 in4

a = 40

b = 10

L = 600

Calculated information for beam:

Mass = 13.447 slugs

Kx = 2715.9 lb/in

Ky = 941.4 lb/in

J = 3923.538 in4

Fundamental modes for beam:

First bending mode, weak axis - 2.678 Hz

First bending mode, strong axis - 4.550 Hz

First torsional mode - 42.853 Hz

s

t

u

v

Mode 40 - The first torsional mode for the beam, predicted frequency, 45.020 Hz. Torsional mode is evident from deflection plots.

Mode 37 - A harmonic mode for the side wall

• Select Additional Modes, between 40 and 50 Hz.
• Select Displacements, Translation for Fringe Result.
• Select Displacements, Translation for Deformation Result.
• Click -Apply- to display fringe plot.

The maximum error in predicted modes is 5% from the analysis. The analyst knows from other models checked for the analysis that most of this error is mesh dependent. For a final analysis, which is not run-time limited, errors of less than 2% could be expected.

Step 14. Fields: Create / Non Spatial / Tabular Input

a

e

b

sawtooth

c

d

f

g

• Create Fields
• Fields: Create / Non Spatial / Tabular Input.
• Enter sawtooth as Field Name.
• Select time as the independent variable.
• Open the input data page.
• Input the data.
• Press OK to close form.
• Click –Apply-.

a

b

modal_dynamic

c

d

• Enter modal_dynamic as Load Case name.
• Select Time-Dependent for Load case type.
• Click -Apply- to create load case.
Step 16. Load/BCs: Create / Force / Nodal

a

f

e

<0, 100, 0>

f:sawtooth

b

c

end_force

g

d

• Loads/BCs: Create / Force / Nodal.
• Ensure modal_dynamic is selected as the load case.
• Enter end_force as Set Name.
• Open Input Data form.
• Enter <0,100,0> as Load Vector.
• Input time dependency on sawtooth waveform.
• Click OK to close form.

j

k

h

i

m

l

• Open the Select Application Region form
• Select the Surface or Face picking icon
• Select Surface 5
• Click OK to exit form.
• Click -Apply- to create force.

a

d

b

e

c

f

• Select Displ_wall and Force_end_force.
• Click OK to apply and close form.
• Click -Apply- to modify load case.
Step 18. Analysis: Analyze / Entire Model / Full Run
• Setup Analysis.
• Analysis: Analyze / Entire Model / Full Run.
• Input modal_dynamic_job1 as Job Name.
• Open the Load Step Creation form.

a

b

modal_dynamic_job1

c

g

h

modal_dynamic

d

i

e

f

• Enter modal_dynamic as Job Step Name.
• Select Transient Dynamic as Choose Solution Type.
• Open the Solution Parameters form.
• Choose Linear as Linearity.
• Select Modal Time Integration.
• Open Load Increment Parameters form.

n

o

j

1

k

5

0.05

• Enter 1 as Time Step.
• Enter 5 as Total Time.
• Click OK to close form.
• Open Select Load Case form.
• Select modal_dynamic.
• Click OK to close form.
• Click -Apply-.
• Click Cancel to close Step Create form.

l

m

p

q

s

t

r

u

v

It is necessary to perform a modal analysis prior to performing a modal_dynamic analysis so that the relevant modes have been extracted. Unlike some packages, the load vector considered for the dynamic analysis does not have to be applied for the modal step.

• Open Load Step Selection form.
• Select modal andmodal_dynamic in the order indicated to run analyses.
• Deselect Default Static Step.
• Click OK to close form.
• Click -Apply- to launch analysis.
Step 19. Analysis: Monitor / Job

a

b

modal_dynamic_jo

c

Case # Indicates which load step is being solved.

Time step for solution.

• Monitor the Job.
• Monitor / Job.
• Select modal_dynamic as Job Name.
• Open View Status File form.

Total time solved.

Step 20. Analysis: Read Results / Results Entities / Attach

a

b

modal_dynamic_jo

c

• Attach the Result file.
• Read Results / Results Entities / Attach.
• Select modal_dynamic_job1 as Job Name.
• Click Apply to read results.
Step 21. Results: Read Results / Graph / Y vs. X

a

b

• Post-process the results.
• Results: Read Results / Graph / Y vs. X.
• Select modal_dynamic as Case.
• Select modal_dynamic as Case.
• Click Filter to select full results set.
• Click Apply to close selection form.
• Close the form by clicking Close.

c

d

f

e

k

m

Node 340

g

n

h

i

j

l

• Select Displacement, Translation for Result.
• Select Y-Component for Quantity.
• Select Global Variable for X.
• Select Time for Variable.
• Select pick target form.
• Select the Node picking icon.
• Select Node 340, the center top node on the free end (the node number might be different).
• Click -Apply- to close form and create plot.
Step 22. Results: Create / Quick Plot

a

b

f

c

d

e

• Create a quick plot.
• Create / Quick Plot.
• Select time of 1.3 sec.
• Select Displacement, Translation for Fringe.
• Select Displacement, Translation for Deform.
• Click Apply to create plot.
• Continue through timesteps to establish time of maximum displacement.

Maximum Displacement occurs at time t=1.3 sec. At a magnitude of 0.532”

g

h

i

j

• Select 1.3 sec for time.
• Select Stress, Global System for Fringe.
• Select Von Mises for Quantity.
• Click -Apply- to create plot.

Maximum Displacement occurs at t=1.3 sec, since primary stress is bending, the maximum stress will also occur at this time. Evident from the plot above, the maximum stress is 2,61 ksi, occurring at the fixed position

a

d

b

linear_dynamic

c

e

f

• Enter linear_dynamic as Case Name.
• Select Displ_wall and Force_end_force.
• Click OK to close form.
• Click -Apply- to create load case.
Step 24. Analysis: Analyze / Entire Model / Full Run

g

a

h

d

linear_dynamic

e

f

b

Sawtooth_linear_j

c

• Analysis: Analyze / Entire Model / Full Run.
• Enter sawtooth_linear_job1 as Job Name.
• Open Load Step Creation form.
• Enter linear_dynamic as Job Step Name.
• Select Transient Dynamic for Solution Type.
• Open Solution Parameters form.
• Select Linear for Linearity.
• Select Direct for Time Integration.

Keep working on Solution Parameters form in next page

j

0.05

k

5

l

0.5

m

0.25

i

o

n

Gamma and Beta are operators for the Newmark time integration method. As we are using the single step Houbolt method, we can input the default values

• Open the Load Increment Parameters form.
• Enter 0.05 as Time Step Size.
• Enter 5 as Total Time.
• Enter 0.5 as Gamma (default).
• Enter 0.25 as Beta (default).
• Click OK to Close Increment Parameters form.
• Click OK to close Solution Parameters form.

q

r

p

t

s

• Open the Select Load Case form.
• Select the linear_dynamic for Load Case.
• Click OK to close Select Load Case form.
• Click -Apply- to create Load Step.
• Click Cancel to close the form.

v

w

x

• Open the Load Step Selection form.
• Select the linear_dynamic Load Case.
• Deselect the Default_Static_Step.
• Click OK to close Step Select form.
• Click on Job Parameters
• Switch on Use Tables
• Click OK
• Click -Apply- to launch analysis.

Job Parameters..

y

u

z

bb

aa

Step 25. Analysis: Read Results / Results Entities / Attach

a

Sawtooth_linear_jo

b

c

Attach the Result file.

• Read Results / Results Entities / Attach.
• Select sawtooth_linear as Job Name.
• Click -Apply- to read results.

Step 26. Results: Create / Graph / Y vs. X

a

b

c

e

d

• Post-process the results.
• Results: Create / Graph / Y vs. X.
• Select linear_dynamic as Result Case.
• Click Filter to sort results.
• Click -Apply- to read results.
• Close the form by clicking Close.

j

l

Node 340

f

g

h

i

m

k

• Select Displacement, Translation for Result.
• Select Y-Component for Quantity.
• Select Global Variable for X.
• Select Time for Variable.
• Select pick target form.
• Select the Node picking icon.
• Select Node 340, the center top node on the free end (the node number might be different).
• Click -Apply- to close form and create plot.
Step 27. Results: Create / Quick Plot

a

b

f

c

d

e

• Create a quick plot.
• Create / Quick Plot.
• Select time of 1.25 sec.
• Select Displacement, Translation for Fringe.
• Select Displacement, Translation for Deform.
• Click -Apply- to create plot.
• Continue through timesteps to establish time of maximum displacement.

Maximum Displacement occurs at time t=1.25 sec. At a magnitude of 0.538”

g

h

i

j

• Select 1.25 sec for Result Cases.
• Select Stress Global System for Fringe.
• Select Displacement, Translation for Deformation.
• Click -Apply- to create plot.

Maximum stress at time of peak displacement 2.63 ksi