ANSYS Mechanical-APDL Harmonic Analysis Example and Comparison to ANSYS Mechanical results

Size: px

Start display at page:

Download "ANSYS Mechanical-APDL Harmonic Analysis Example and Comparison to ANSYS Mechanical results"

Tyrone Newton
6 years ago
Views:

1 ANSYS Mechanical-APDL Harmonic Analysis Example and Comparison to ANSYS Mechanical results Dave Johnson Penn State Erie 9/11/2017 1

2 Disk modal and harmonic analyses Steel disk - 75 mm radius and 3mm radius center hole, and 0.34 mm thickness 1421 SHELL 181 elements Modulus = 200,000 Mpa Poisson s Ratio = 0.3 Density = 7.85E-9 tonnes/mm 3 TOTAL MASS: 0.471E-04 (tonne) Support: simply-supported, (no translation: UX = UY = UZ = 0) at the edge of the hole 9/11/2017 2

3 Hand calc for verification and validation of modal analysis results Reference: Mark s Standard Handbook for Mechanical Engineers, 8th ed., p For a flat circular plate constrained at the center, the umbrella mode (zero nodal diameters) is predicted by: Where: E = elastic modulus (N/mm 2 ) r = plate radius (mm) g = gravity acceleration (mm/s 2 ) ν = Poisson s ratio t = plate thickness (mm) 9/11/2017 3

RANGE REQUESTED= 0.00 500.00 1 31.02836452595 2 31.15668930275 3 53.

4 Hand calc for verification and validation of modal analysis results *** FREQUENCIES FROM BLOCK LANCZOS ITERATION *** MODE FREQUENCY (HERTZ) FREQUENCY RANGE REQUESTED= /11/2017 ~3.2% difference Hand calc vs. FEA 4

5 Modal Analysis Results *** FREQUENCIES FROM BLOCK LANCZOS ITERATION *** 9/11/2017 MODE FREQUENCY (HERTZ) FREQUENCY RANGE REQUESTED= In the frequency range of interest, we observe 14 modes: 31 < f n < 497 Hz 5

6 Harmonic Analysis Setup Method: Mode Superposition Load (1 N) on keypoint in z-direction at edge (at 3 o clock position) use all (14) modes from 0 to 500 Hz, solve 100 substeps 0.03 damping ratio (minimal, structural value) perform an expansion pass after the harmonic analysis solution 9/11/2017 6

7 Harmonic Analysis Results Z-deformation at node where the harmonic load is applied Linear vs. Log? Note: the Mode Superposition Solution used 14 modes (in range Hz), and max. amplitude (27.59 mm) 30 Hz 9/11/2017 7

8 Harmonic Analysis Results - 2 Use modes from twice the range of interest, i.e., Hz (26 modes were found) Note: the Mode Superposition Solution used 26 modes (in range Hz), and max. amplitude (27.62 mm) 30 Hz 9/11/2017 8

9 Harmonic Analysis Results - 3 Used the FULL Method, not Mode Superposition Note: the FULL Method Solution, maximum amplitude (33.07 mm) 30 Hz 9/11/2017 9

10 ANSYS Mechanical Comparison Modal linked to Harmonic (B-C) vs. Harmonic (D & E) Structural Steel properties from WB library Same geometry, constraint, and loading Similar mesh: 1433/1422 SHELL181 elements TOTAL MASS = E-04 (tonne) [same as ANSYS Mechanical APDL model] 9/11/

11 ANSYS Mechanical Comparison Modal linked to Harmonic (B-C) vs. Harmonic (D & E) (Split to make vertex for loading) 9/11/

ANSYS Mechanical Comparison Modal linked to Harmonic (Schematic Objects B-C) Compared to ANSYS Mechanical APDL Results: *** FREQUENCIES FROM BLOCK LANCZOS ITERATION *** MODE FREQUENCY (HERTZ)

12 ANSYS Mechanical Comparison Modal linked to Harmonic (Schematic Objects B-C) Compared to ANSYS Mechanical APDL Results: *** FREQUENCIES FROM BLOCK LANCZOS ITERATION *** MODE FREQUENCY (HERTZ) FREQUENCY RANGE REQUESTED= /11/

for Amplitude, Solution used 14 modes (in range 0 500

13 ANSYS Mechanical Comparison Modal linked to Harmonic (Schematic Objects B-C) Note: (default) uses log scale for Amplitude, Solution used 14 modes (in range Hz), and max. amplitude (18 mm) 30 Hz 9/11/

for Amplitude, Solution used 26 modes (in range 0 1000

14 ANSYS Mechanical Comparison Harmonic without Modal (Schematic Object D) Note: (default) uses log scale for Amplitude, Solution used 26 modes (in range Hz), and max. amplitude (26 mm) 35 Hz 9/11/

damping input under Analysis Settings (α = 11 and β = 2e-5)

15 ANSYS Mechanical Comparison Harmonic without Modal (Schematic Object E) using FULL Method NOTE: different damping input under Analysis Settings (α = 11 and β = 2e-5) see next slide, and max. amplitude (18.2 mm) 30 Hz 9/11/

16 Full Harmonic, Damping Input From ANSYS Help > Mechanical APDL > Structural Analysis Guide > Alpha & Beta Damping (Rayleigh Damping) For this example: 9/11/

17 Comparing Results 9/11/

18 Comparing Results 9/11/

19 Comparing Results Maximum Response occurs at 30 or 35 Hz and the Next Highest Response occurs at 80 Hz 9/11/

20 Conclusions/Observations Mechanical (WB) default method for Harmonic Analysis is Mode Superposition. The ANSYS default method is Full Mechanical (WB), Harmonic Analysis without linked Modal Analysis, uses 2x the user-requested frequency range, i.e., requested Hz, and WB used modes from Hz Mechanical (WB), default Frequency Response plot format uses a log scale for the y-axis (for the Amplitude) 9/11/

21 Why? Conclusions/Observations Does the Full Method show higher max. values, in general? Is Mechanical MSUP-26 max. value at 35 Hz? Should we care about variations at higher frequencies where the amplitude is much less? 9/11/

22 finish /clear /PREP7 ET,1,SHELL181! use 3D 4-node thin shell element!* MPTEMP,,,,,,,, MPTEMP,1,0 MPDATA,EX,1,,200000! modulus in MPa MPDATA,PRXY,1,,0.3! Poisson's ratio MPTEMP,,,,,,,, MPTEMP,1,0 MPDATA,DENS,1,,7.85e-9! density in tonnes/mm^3 sect,1,shell,, secdata, 0.34,1,0.0,3! shell thickness 0.34 mm secoffset,mid seccontrol,,,,,,, PCIRC,75,3,0,360,! 75 mm outer radius, 3 mm radius center hole SMRT,6! Smart size for meshing ESIZE,5,0,! Global element size MSHAPE,0,2D! MSHKEY,0! allow "free" meshing!* AMESH,all! create the mesh FINISH /SOLU ANTYPE,2! Modal analysis MODOPT,LANB,50! use (default) Block Lanczos method EQSLV,SPAR MXPAND,50,,,0! extract & expand up to 50 modes LUMPM,0 PSTRES,0!* MODOPT,LANB,50,0,500,,OFFbv! frequency range Hz lsel,s,,,5,8,1 DL,all,,UX, DL,all,,UY, DL,all,,UZ, lsel,all solve save,disk_modal,db finish! constraints on edge of hole /POST1 set,list finish

23 /SOLU ANTYPE,3!* HROPT,MSUP,,,0 HROUT,ON LUMPM,0!* HROPT,MSUP,14,1,0 HROUT,ON,OFF,0!* FK,1,FZ,1, HARFRQ,0,500, NSUBST,100, KBC,1!* ALPHAD,0, BETAD,0, DMPRAT,0.03, DMPSTR,0, MDAMP,1,,,,,,,!* solve finish save,disk_harmonic,db /SOLU!* EXPASS,1 NUMEXP,ALL,0,500,1 HREXP,ALL,!* SOLVE! Harmonic Analysis! Mode Superposition Method! use (all) 14 modes from modal analysis! Harmonic load amplitude! Frequency range! substep thru freq range! step change boundary conditions! 3% damping ratio! Harmonic Analysis Expansion Pass! Frequency range /POST26! Time History Postprocessor *GET,nn,KP,1,ATTR,NODE NSOL,2,nn,U,Z,!* LINES,200 PRCPLX,1! print Amplitude/Phase vs. Real/Imaginary results /AXLAB,Y,UZ Deformation (mm) /title, disk harmonic analysis - w/linear y-axis (default) plvar,2 prvar,2 /GROPT,LOGY,ON /title, disk harmonic analysis - w/log y-axis to match WB plvar,2

Modal Analysis of a Beam (SI Units)

APPENDIX A Modal Analysis of a Beam (SI Units) Objectives Perform normal modes analysis of a cantilever beam. Submit the file for analysis in MSC/NASTRAN. Find the first three natural frequencies and mode