Do the displacement Ux in ANSYS modal analysis is real displacement? 4

[richard98]

Hello all,

I am confused with the meaning of displacement Ux in ANSYS modal analysis.

In my modal analysis, the maximum length of the model is no more than 11e-3 m, but the modal results of first mode in ANSYS plotted that DMX = 149.608. The system of units of my model is SI, so do the DMX means the maximum nodal displacement is 149.608 m? But I think it is impossible.

What do the maximum nodal displacement DMX really mean?
Do the displacement Ux in ANSYS modal analysis is real displacement? Or does it just mean the realative displacement?

Thanks in advance.

Richard

Below is my batch commands of the model, where epoxy is sandwiched by two Kovar blocks:

/prep7

/com ---------------------
ET,1,solid45 !Brick

! Epoxy
mp,DENS,1, 1.8e3
mp,EX,1, 2e9 !E = 2 GPa
mp,NUXY,1, 0.3


! Kovar
mp,DENS,2,8.36e3
mp,EX,2,140e9 !E= 140GPa
mp,NUXY,2,0.32

bi_hou = 2.5e-3
nei_Y = 5e-3
nei_x = 6e-3
nei_gao = 3e-3


block,0,bi_hou,0,nei_y,0,nei_gao
block,bi_hou, bi_hou + nei_x,0,nei_y, 0, nei_gao
block,bi_hou + nei_x, bi_hou + nei_x + bi_hou, 0,nei_y, 0, nei_gao

alls
vglue,all

alls
vsel,s,loc,x,bi_hou, bi_hou + nei_x
vatt,1,,1

alls
vsel,u,mat,,1
vatt,2,,1

alls
vmesh,all

/solu
alls

ANTYPE,2
MODOPT,LANB,5,,,,off
MXPAND,5,,,no


alls
asel,s,loc,z,0
DA,all,all,0 !Bottom suface

alls
asel,s,loc,z,nei_gao
DA,all,UZ,0 !Top suface

alls
asel,s,loc,y,0
asel,a,loc,y,nei_y
DA,all,uy,0 !Side sufaces

alls
solve
save,_solve,db

finish


/eof

 

[pja]

It's a relative displacement.

 

[GregLocock]

As pja said. Usually it is scaled so that the largest amplitude is a certain figure (often 1) or so that the modal mass is unity, but there are other variations.

In order to get 'real life' displacements you need to add damping, for each mode, and an excitation spectrum.

You get the same probelm with experimental modal analysis, there are several different scaling decisions that can be made.

Cheers

Greg Locock

 

[Drej]

In ANSYS plotting the mode shape of a mode via the pldisp,, family of commands results from either:

1) the mode being shown in terms of the modal mass matrix where:

PSI(transpose)*[M]*PSI = 1 = modal mass matrix

i.e. plotting of the eigenvectors in terms of the modal mass matrix ("MASS NORMALISED&quot. This is the default in ANSYS.

2) the mode being shown normalised to unity ("UNIT NORMALISED&quot. The unit value is taken as the largest component of the eigenvector(s).


(1) or (2) above can be set using the following command:

MODOPT, Method, NMODE, FREQB, FREQE, PRMODE, Nrmkey, , Cekey

by setting the "Nrmkey" to either off (default) or on (unity). Be careful if you normalise to unity, as ANSYS will need to use the mass normalised matrix if a subsequent spectrum analysis is carried out.

-- drej --

 

[richard98]

As drej mentioned above,

PSI(transpose)*[M]*PSI = 1 = modal mass matrix

Do the PSI means the mode shape, i.e., the eigenvectors?

Another important question:
I get different maximum displacement(DMX) for the first mode with different material property, e.g., modulus EX, so can I plot the curve of DMX vs. EX to show the relationship between DMX and EX?


Thank you very much!

Richard

 

[elogesh]

Hai,

It is better to do harmonic response analysis and plot the maximum displacement w.r.to Material property.
If it is pure tone(single frequency), then Graph is 2D.
If it is frequency sweep,then graph is 3D.

Mode shape and eigen vectors are same.

Regards,

 

[Drej]

Richard,

PSI (the greek letter "PSI&quot is a matrix of eigenvectors i.e.

Capital PSI = [{little psi,1} {little psi,2} ... {little psi,n}] = [{little psi(11)} {little psi(12)}... {little psi(1n)} ]

in the equation given in my previous reply, the PSI in question is Capital PSI. The little psi are column matrices for each mode as shown.

-- drej --