No stress in PSD Analysis results

[JamesDE2008]

I am performing a PSD analysis in Ansys9.0 for an electronic housing by defining a based excited PSD loading G^2/Hz in acceleration. The housing was fixed through four brackets to vibration desk, however I can not find any stress in loadstep 3 to 5. I can only find displacement in resultant 1.7 and in x,y,z direction 0.9999. The displacement is also constant in total model except in the area of brakets the displament shows from zero to 1.7 (or 0.9999 for compoment displacement). Can some people to tell me, what could be the problem and how should I understand this. Actually in loadstep Modal analysis and PSD analyse the element stress output has been already selected.
This is my code:

!!! FE Model has been already constraint in bottom of four brakets.

/SOLU
ANTYPE,MODAL?
MODOPT,LANB,100,0,2000,?,OFF,?,0
LUMPM,1
PSTRES,0
SOLVE
FINISH

/SOLU
ANTYPE,MODAL?
EXPASS,ON
MXPAND,100,,,YES,?
SOLVE
FINISH

/SOLU
ANTYPE,SPECTR
SPOPT,PSD,,YES

PSDUNIT,1,accg,9800!mm,mpa,t, unit system

psdfrq,1,,1,10,20,80,400,2000
psdval,1,2.2e-2,2.2e-2,2.4e-3,2.4e-3,1.2e-4

NSEL,R,LOC,y,0

D,ALL,uy,1.0!Ux,Uy,Uz already constraint and now PSD loading applied also here.

ALLSEL,ALL
PFACT,1,BASE
PSDRES,DISP,ABS
PSDRES,VELO,ABS
PSDRES,ACEL,ABS
SOLVE
FINISH
/SOLU
ANTYPE,SPECTR
PSDCOM,0.005,100!or PSDCOM,0.0001,100
SOLVE
FINISH

/POST1
SET,LIST
SET,FIRST?
PRNSOL,DOF?
PRESOL,ELEM?
PRRSOL,F?
set,,,1,,,,103

FINISH


Hope somebody can help! many thanks!

 

[Transient1]

Maybe I'm missing something, but I don't see more than 1 load step in the commands you have listed here. Why are you worried about load steps 3 to 5? What results do 1 and 2 show you. Perhaps, you are missing some information about your problem. I would triple check your constraints and not apply them twice.

 

[JamesDE2008]

Thanks for the advice!

I realised that my FE model probably was built too stiff, because the joints (screws and rivets)in my model mostly were simplified through VGLUE or CPs. I did a test calculation with reduced structure and then I can get stress and displacement in final loadstep. So I guess that my FE model probably too stiff and the total structure behaviours like a complete parts, so I can not find stress.

I will review my FE model and do further test calculations. Any way I will back again here.

Does any one know can we receive the stress and displacement directly in post1 in ansys9.0. How should we interpret the stress and displacement, which caution should we pay?!

 

[Transient1]

Check the theory guide and structural guide for ANSYS for your questions about stress and displacement from a PSD analysis. The stress is calculated using an algorithm called segalman-reese and the displacment can be either absolute displacement or relative to the base. You should post process in post26 for the PSD analysis. Again, the documentation covers all these questions.

First of all it sounds like you haven't made a simple test case to figure out everything before you moved on to a more difficult problem. I highly suggest taking that approach.

Secondly, you should have run a modal analysis and reviewed those results before running a PSD model. If the first mode of your structure occurs above 4000 Hz and the PSD curve goes from 20 to 2000 Hz, then it is not unreasonable to have very little stresses, possibily zero.

 

[JamesDE2008]

Thanks for the advice from Transient1!

I changed LUMPM,1 into LUMPM,0 and looked the results in loadstep 3 and then I received reasonable displacement and stress. Anyone can tell me, why should we look the results in loadstep 3, how is about result from loadstep 4 and 5?

As I know, the stress and displacement from loadstep 3 is 1 sigma value, for the margin of safety should we convert 1 sigma stress into 3 sigma stress? Should we do the same thing for displacement?

Hope anyone can help me,thankls a lot!

 

[jgeren]

Step 4 is velocity and step 5 is acceleration. They are all 1 sigma values. No stresses of use in either step. I don't even know if they are calculated as they are useless. I'm almost positive equivalent stress is the only usefull stress from PSD.