Learning Forum

[biao.zhou]

I have got a harmonic mode superposition result and it is saved as a .rfrq file. But when I close ANSYS and open the .db result again, in general postproc (/post1) I can only load the .rst file and see modal analysis result, only in /post26 I can load the .rfrq file and get amplitude-frequency plot, but in /post26 I can't get contours to watch the whole component.

I want to know how can I get the contours by MSUP result, and how can I export data(displacement, stress,etc) from the harmonic response result.

[Chandra Sekaran]

You will need to do an expansion pass after the mode superposition analysis to create a rst file for the harmonic analysis as outlined in section 4.6.3 of the structural analysis guide at https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/ans_str/Hlp_G_STR4_MODESUPER.html
Section 4.6.5 also provides the below example that includes the expansion pass.
4.6.5. Example: Mode-Superposition Harmonic Analysis
! Build the Model
/FILNAM,... ! Jobname
/TITLE,... ! Title
/PREP7 ! Enter PREP7
---
--- ! Generate model
---
FINISH

! Obtain the Modal Solution
/SOLU ! Enter SOLUTION
ANTYPE,MODAL ! Modal analysis
MODOPT,LANB ! Block Lanczos
MXPAND,,,,YES. ! Expand and calculate element results
D,... ! Constraints
SF,... ! Element loads
SAVE
SOLVE ! Initiate modal solution
FINISH

! Obtain the Mode-Superposition Harmonic Solution
/SOLU ! Enter SOLUTION

ANTYPE,HARMIC ! Harmonic analysis
HROPT,MSUP,... ! Mode-superposition method; number of modes to use
HROUT,... ! Harmonic analysis output options; cluster option
LVSCALE,... ! Scale factor for loads from modal analysis
F,... ! Nodal loads
HARFRQ,... ! Forcing frequency range
DMPRAT,... ! Damping ratio
MDAMP,... ! Modal damping ratios
NSUBST,... ! Number of harmonic solutions
KBC,... ! Ramped or stepped loads
SAVE
SOLVE ! Initiate solution
FINISH

! Review the Results of the Mode-Superposition Solution
/POST26
FILE,,RFRQ ! Postprocessing file is Jobname.rfrq
NSOL,... ! Store nodal result as a variable
PLCPLX,... ! Define how to plot complex variables
PLVAR,... ! Plot variables
FINISH

! Expand the Solution (for Stress Results)
/SOLU! Re-enter SOLUTION
EXPASS,ON ! Expansion pass
EXPSOL,... ! Expand a single solution
HREXP,... ! Phase angle for expanded solution
SOLVE
FINISH

! Review the Results of the Expanded Solution
/POST1
SET,... ! Read results for desired frequency
PLDISP,... ! Deformed shape
PLNSOL,... ! Contour plot of nodal results
---
FINISH