Problems with MCOM file for the spectral analysis 1

[aldotoscano]

Hi!!!

I'm having trouble reading the MCOM file from the POST1 for the spectral analysis. I do READ INPUT FROM but the only results that I see are the EXPANDED/CALCULATE ELEMENTS that result from the modal analysis, but no spectral data. Could somebody help me?

I think I'm doing all previous operations correctly, because I am able to generate the MCOM file.

Thank you very much!

Yours truly,

Aldo Toscano

 

[Drej]

I'm not sure I understand you correctly. How do you know that these results are "modal results" and not spectral? By "results" do you mean stresses, displacements, forces...?

I presume you've taken a route as follows:

1/ carried out a modal analysis to extract the required modes (including expansion of the modes) and then

2/ applied your spectral loading using the SV-FREQ input and then solved for this.

3/ combine the results of the the modal directions (all of X, all of Y, all of Z) using CQC for example (this is where you input your MCOM file), and then

4/ finally cross-combining the modes using SRSS (for example)


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[aldotoscano]

Thanks Drej!

I'm taking the exact steps of the ANSYS Structural Analysis Guide. The problem is, that I plot results (contour/nodal solution) displacements and stresses (expanded modes, remember?) for the modal results; then, after following the spectrum analysis route I get exactly the same displacements and stresses as in the modal analysis (I'm aware that these are not "real" displacements and stresses since these are modal expanded results). Like if ANSYS never read the MCOM file, or the MCOM file wasn't created correctly.

I'm using PIPE 20, MASS 21, SHELL 63 and SOLID 45 elements. Constraint equations, some nodes with zero displacement, the material is copper, SPRS for the spectrum solution, SRSS for the mode combination and that's pretty much it.

 

[Drej]

Are you reading in the correct results? After you do a solve for the spectrum analysis, do you save this as a separate results file and then read this in? The ANSYS example isn't very clear in the help file, and it is very simple (only a single direction). Are you using this sample as your reference?

To be honest there are too many questions that need to asked to find out the problem - it could be numerous things. If you can you post your model macro, including the /mcom file it would make it easier though.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[aldotoscano]

Thanks again Drej!!!

Yes, I'm using the ANSYS example as reference, and you are right, it is not very clear. The RST file is generated after the modal analysis (expanded and calculated results) is performed but then, after I run the spectrum I do not save any file.

If you think it would help, I could send you the macro (it would take me a couple of hours).

Yours truly,

Aldo Toscano

 

[Drej]

Try this. I have amended the example which should make things clearer.

! -----------------
!
! ANSYS example spectrum analysis
fini
/cle
/filnam,example_spectrum

/PREP7
/TITLE Seismic Response of a Beam Structure

ET,1,BEAM3
R,1,273.9726,(1000/3),14 ! A = 273.9726, I = (1000/3), H = 14
MP,EX,1,30E6
MP,DENS,1,73E-5
K,1
K,2,240
L,1,2
ESIZE,,8
LMESH,1
NSEL,S,LOC,X,0
D,ALL,UY
NSEL,S,LOC,X,240
D,ALL,UX,,,,,UY
NSEL,ALL
save
FINISH

/SOLU
ANTYPE,MODAL ! Mode-frequency analysis
MODOPT,lanb,10,,, ! *****block lanczos extract 10 modes
MXPAND,10,,,YES,0.005 ! *****
M,ALL,UY
OUTPR,all,1 ! ***** all
SOLVE
save
FINISH

/SOLU
ANTYPE,SPECTR ! Spectrum analysis
SRSS,0.15,DISP ! ********* use SRSS combination
SPOPT,SPRS ! Single point spectrum
SED,,1 ! Global Y-axis as spectrum direction
SVTYPE,3 ! Seismic displacement spectrum
FREQ,.1,10 ! Frequency points for SV vs. freq. table
SV,,.44,.44 ! Spectrum values associated with frequency points
SOLVE
save
FINISH

! ********* all this has changed
/post1
/title,MODAL COMBINATION
/input,,mcom
alls
rappnd,2
save
fini

/post1
set,2,1
!
! END OF FILE
! ---------------------------


Post your macro if you can also.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[aldotoscano]

Many many thanx Drej!!! I'll try it and keep you notify...

Greetings,

Aldo

 

[aldotoscano]

Drej,

I tried with your macro with the same results... again, only the modal results (stress and displacements) but no combination with spectrum results.

Here is the macro that I was using before you post yours:

/SOL
ANTYPE,2
MSAVE,0
MODOPT,LANB,5
EQSLV,SPAR
MXPAND,5, , ,1
LUMPM,0
PSTRES,0
MODOPT,LANB,5,0,0, ,OFF
SOLVE
FINISH
/POST1
SET,LIST
SET,FIRST
ANMODE,10,0.5, ,0
AVPRIN,0, ,
FINISH
/SOLU
ANTYPE,8
SPOPT,SPRS,5,1
OUTRES,ALL,ALL,
ERESX,DEFA
SVTYP,3,1,
SED,0,1,0,
ROCK,0,0,0,0,0,0,
FREQ,262.67,325.79,338.41,468.74,662.35,0,0,0,0
SV,0.02,0.14,0.14,0.14,0.14,0.14,0.14,
SPTOPT
SRSS,0.001,DISP
SOLVE
FINISH
/POST1
sumtype,prin
/INPUT,'228_cable_actual_definitivo','mcom','C:\DOCUMENTS AND SETTINGS\ADMINISTRATOR\MY DOCUMENTS\PROYECTOS\Pruebas para conector VW\Actual\Espectral\Modificado\',, 0



and the MCOM file as requested:

/COM,ANSYS RELEASE 7.0 UP20021010 15:15:08 06/08/2005
/COM, 228_cable_actual_definitivo.mcom
LCOPER,ZERO
LCDEFI,1, 1, 1
LCFACT,1, 0.151070E-10
LCASE,1
LCOPER,SQUARE
LCDEFI,1, 1, 2
LCFACT,1, 0.398005E-10
LCOPER,ADD,1,MULT,1
LCDEFI,1, 1, 3
LCFACT,1, 0.584116E-10
LCOPER,ADD,1,MULT,1
LCDEFI,1, 1, 4
LCFACT,1, 0.298334E-10
LCOPER,ADD,1,MULT,1
LCDEFI,1, 1, 5
LCFACT,1, -0.222800E-10
LCOPER,ADD,1,MULT,1
LCOPER,SQRT

I have the FE model macro but it's quite large, if you need it I could email it to you.

Thanks again! I hope these helps!!

Greetings,

Aldo

 

[aldotoscano]

Dear Drej:

I ran your whole macro, with the beam model (not for my model but for the beam example) and it's the same...POST01 plots the same displacements as the modal results with no change for the Spectrum analysis.

Thanks!

Aldo

 

[Drej]

I've checked my macro and it works fine. Use my macro and go into /Post1 and read in results set,2,1 - these are the spectrum results. Compare these with set,1,1. To do this you should run my macro and then type:

/post1
set,2,1 ! spectrum results
pldisp

set,1,1 ! first mode shape
pldisp

and compare the two. Tell me exactly how you're postprocessing (the sequence, the commands). Below is the comparison:

set,1,1
PRNSOL,U,COMP

NODE UX UY UZ USUM
1 -0.37132E-22 0.0000 0.0000 0.37132E-22
2 0.0000 0.0000 0.0000 0.0000
3 -0.35799E-22 0.78109E-01 0.0000 0.78109E-01
4 -0.22089E-22 0.14433 0.0000 0.14433
5 0.21446E-23 0.18857 0.0000 0.18857
6 0.20461E-22 0.20411 0.0000 0.20411
7 0.38585E-22 0.18857 0.0000 0.18857
8 0.40737E-22 0.14433 0.0000 0.14433
9 0.24302E-22 0.78109E-01 0.0000 0.78109E-01


set,2,1
PRNSOL,U,COMP

NODE UX UY UZ USUM
1 0.20300E-14 0.0000 0.0000 0.20300E-14
2 0.0000 0.0000 0.0000 0.0000
3 0.19888E-14 0.29437 0.0000 0.29437
4 0.18672E-14 0.42511 0.0000 0.42511
5 0.16709E-14 0.52420 0.0000 0.52420
6 0.14088E-14 0.60119 0.0000 0.60119
7 0.10966E-14 0.52420 0.0000 0.52420
8 0.75010E-15 0.42511 0.0000 0.42511
9 0.38116E-15 0.29437 0.0000 0.29437


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[aldotoscano]

Drej,

I followed your steps and you were right... I was able to see the spectrum results, but please correct me if I'm wrong; shouldn't I be able to see the results for all extracted modal forms? I mean, for each substep?

The example extracts 10 modes, shouldn't I be able to see spectrum results for each mode?

What I was doing in the POST01 was incorrect, because I didn't set loadstep 2; I was "looking" only at loadstep 1 results and via GUI READ RESULTS/FIRST SET, NEXT SET.... then CONTOUR PLOT/NODAL SOLU/DISP OR SEQV, so I was looking at the modal results.

I would like to see spectrum displacements and SEQV for each mode, but I can't figure a way to do so. Could you help me?

Thanks again!

Sincerely,

Aldo