## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Modal analysis results affected by local of elements

• Moustafa El-Sawy
Subscriber

I am running a quick test on the modal analysis of a block of concrete supported on four corner nodes on ANSYS apdl. Code is below:

/CLEAR               ! Clear all previous data and start fresh
/PREP7               ! Enter preprocessor phase

! Element Definitions
ET, 1, SOLID185      ! Define SOLID186 element type for solid modeling

! Material Properties for the Solid
MP, EX, 1, (32836.56803/1000)/0.83   ! Define Young's Modulus for solid after adjusting value
MP, PRXY, 1, 0.2     ! Define Poisson's Ratio for the solid
MP, DENS, 1, (23.544/9810.0)/10**9   ! Define Density for the solid after adjusting value
MP, ALPX, 1, 10E-006 ! Define Coefficient of Thermal Expansion for the solid

! Geometry Creation
BLC5, 20000, 20000, 40000, 40000, 50000  ! Create a block starting from origin with the given dimensions

! Meshing Settings for the Solid Block
TYPE, 1               ! Set the element type to SOLID186
MAT, 1                ! Set the material type to the first defined material (for solid)
ESIZE, (5000)         ! Set the mesh size
VMESH, ALL            ! Mesh the created volume

NSEL,S,NODE,,1
NSEL,A,NODE,,2
NSEL,A,NODE,,10
NSEL,A,NODE,,18

D,ALL,UX,0
D,ALL,UY,0
D,ALL,UZ,0

! Re-select everything for subsequent commands
ALLSEL, ALL

/SOLU                           ! Enters the solution processor

DAMPING_RATIO = 0.00            ! Modal Damping Ratio
N_MODES = 25                    ! Number of Modes, When Method = LANPCG, NMODE should be less than 100 to be computationally efficient.

ANTYPE, MODAL                   ! Perform a modal analysis
MXPAND, N_MODES                 ! Number of modes
DMPRAT, DAMPING_RATIO           ! Modal damping ratio
MODOPT, LANB, N_MODES

ALLSEL, ALL
/MKDIR, 'OUTPUT'
/OUTPUT, 'OUTPUT/Modal_Analysis', 'OUT'
SOLVE

FINISH                          ! Exits solution processor /SOLU

We can focus on the rotationalX participation factor printed after the modal analysis. For the above run:

***** PARTICIPATION FACTOR CALCULATION *****ROTX DIRECTION
CUMULATIVE     RATIO EFF.MASS
MODE   FREQUENCY       PERIOD      PARTIC.FACTOR     RATIO    EFFECTIVE MASS   MASS FRACTION   TO TOTAL MASS
1     2.32266       0.43054       0.23966E+06    0.673954    0.574382E+11    0.218964        0.218896
2     2.32266       0.43054      -0.35561E+06    1.000000    0.126456E+12    0.701038        0.481922
3     3.73740       0.26757       0.27703E+06    0.779031    0.767451E+11    0.993603        0.292474
4     5.19118       0.19263        0.0000        0.000000     0.00000        0.993603         0.00000
5     6.13489       0.16300       -13571.        0.038164    0.184179E+09    0.994305        0.701900E-03
6     6.13489       0.16300        37987.        0.106824    0.144304E+10    0.999806        0.549939E-02

If I change the origin of my block to 0,0 by doing this instead: BLC5, 0, 0, 40000, 40000, 50000  ! Create a block starting from origin with the given dimensions, I am noticing my results change. See below results for block created using that command:

***** PARTICIPATION FACTOR CALCULATION *****ROTX DIRECTION
CUMULATIVE     RATIO EFF.MASS
MODE   FREQUENCY       PERIOD      PARTIC.FACTOR     RATIO    EFFECTIVE MASS   MASS FRACTION   TO TOTAL MASS
1     2.32266       0.43054       0.25505E+06    0.739835    0.650502E+11    0.350567        0.350486
2     2.32266       0.43054      -0.34474E+06    1.000000    0.118844E+12    0.991041        0.640326
3     3.73740       0.26757        0.0000        0.000000     0.00000        0.991041         0.00000
4     5.19118       0.19263        0.0000        0.000000     0.00000        0.991041         0.00000
5     6.13489       0.16300        17294.        0.050166    0.299092E+09    0.992653        0.161149E-02
6     6.13489       0.16300        36443.        0.105713    0.132813E+10    0.999810        0.715586E-02

Thats one issue, another is why do my rotational mass participation not match with a software like SAP2000. Is there somethjing special about how ansys deals with rotational mass?

For reference, same model on SAP2000 produces this:

 TABLE:  Modal Participating Mass Ratios OutputCase StepType StepNum Period Frequency UX UY UZ SumUX SumUY SumUZ RX RY RZ SumRX SumRY SumRZ Text Text Unitless Sec Hz Unitless Unitless Unitless Unitless Unitless Unitless Unitless Unitless Unitless Unitless Unitless Unitless MODAL Mode 1 0.380409 2.62875 0.74 0 0 0.74 0 0 0 0.26 0 0 0.26 0 MODAL Mode 2 0.369457 2.706675 0 0.68 0 0.74 0.68 0 0.32 0 0 0.32 0.26 0 MODAL Mode 3 0.232478 4.301482 0 0 1 0.74 0.68 1 0 0 0 0.32 0.26 0 MODAL Mode 4 0.176128 5.677689 0 7.47E-20 5.216E-20 0.74 0.68 1 2.06E-20 4.894E-20 0.99 0.32 0.26 0.99 MODAL Mode 5 0.149814 6.674944 0.26 0 0 1 0.68 1 0 0.73 0 0.32 1 0.99 MODAL Mode 6 0.141023 7.091042 0 0.32 0 1 1 1 0.68 0 0 1 1 0.99

You will notice for the SAP2000 output, it shows most of the rotationalX mass participating in the 6th mode with a frequency of 7.1 Hz while ANSYS is indicating the first 2 modes are the ones with the high rotational X mass participation.

• Dave Looman
Ansys Employee

You have duplicate modes so it's random what direction they will be in.  Only the combination of the duplicate modes will be consistent.  Ansys reports the rotational mass participation about the global origin.  SAP2000 might compute it about the center of mass.

• Moustafa El-Sawy
Subscriber

Hi Dave, thanks for the response. Is there a way to be able to set ansys to report rotational mass participation about the center of mass?

• Dave Looman
Ansys Employee

No, there's no option to do that.  I wanted to add that supporting the model at just the corners produces a lot of local deformation and the results will vary with the mesh size.  A corner has no cross-sectional area so the finer the mesh the greater the local deformation and stress.

• Moustafa El-Sawy
Subscriber

Also regarding the different calculation of mass participation when it comes to rotation. This should give different values but the governing mode for rotation should be the same right? in other words, the mode with the highest mass participation for rotation should be the same accross different software but the values might differ based on how they calculate it?

• Moustafa El-Sawy
Subscriber

Hi Dave, thanks! This is just a test model to illustrate my issue.

Would you be able to take a look at my other post regarding how to apply rotational stiffness to my base of solid elements?

• Dave Looman
Ansys Employee

I don't think the two methods for computing rotational mass participation will necessarily be maximum for the same mode.  I haven't seen your other post, but it sounds like you could just connect a torsional spring to the base nodes.

• Moustafa El-Sawy
Subscriber

How come? doesnt the controlling the frequency for a certain mode of motion have to match between two softwares?

for example the controlling mode for translation in X should match between software otherwise each software will have different behavior in dynamic analysis?

Regarding my other post, im unable to do that because solid elements dont have a rotational DOF at their nodes.

• Mike Rife
Ansys Employee

Hi Moustafa

In the first model all the mass is on one side of the X axis, so all the mass is going in the same direction with respect to rotation about x.  Whereas in the second case half of the mass is on each side of the X axis.  So half of the mass is going positive rotation about X and the other half negative rotation so the cancellation.

In the beginning of troubleshooting it helps to not assume one code is right and the other wrong.  First, compare the theory between the two to make sure that they are computing the same thing.  It could be that there is something defined slightly different, but equally valid approaches, between the two codes.  Have you compared the actual implementation?

Mike

p.s. sory if I am repeating any of the prior discussion...I started replying to this post when there were no replies.  Got sidetracked.  Then finished and when I posted then I was able to see that whole discussion (page refresh).

• Moustafa El-Sawy
Subscriber

Thanks for your reply Mike. I think what was confusing me is I was accustomed to SAP2000 where the mass participation is calculated based on the center of mass compared to ANSYS where everything is defined based on the origin. Is there any way to make it report mass participation based on the center of mass?