Learning Forum

[OliverK]

Hi there,

I'm currently investigating the influence of a new type of bearing on the rotordynamic behavior of a rotor system. What is special about this bearing is that it has unsymmetrical stiffness and damping matrix in X, Y, ROTX and ROTY directions, and sometimes it has negative values of these dynamic properties, which means I cannot just use a general joint to model it. So I turned to creating a MATRIX27 element by inserting an APDL command snippet object. Here is my code, for example, to model the stiffness of the bearing:

/PREP7
! define a node
local,12,0,10,5,5,0,0,0 !CS definition            !  Defines a local coordinate system by a location and orientation.
csys,0 ! Use a specific CS                    !  Activates a previously defined coordinate system.
toffst,273.15,  ! Temperature offset from absolute zero
*GET,NodeJ,NODE,,COUNT
NodeJ = NodeJ + 1
n,NodeJ,0,0,0,0,0,0
d,NodeJ,UX,%_FIX%
d,NodeJ,UY,%_FIX%
d,NodeJ,UZ,%_FIX%
d,NodeJ,ROTX,%_FIX%
d,NodeJ,ROTY,%_FIX%
*GET,KLid,ELEM,,COUNT
KLid = KLid + 1
DOF,UX,UY,UZ,ROTX,ROTY,ROTZ
ET,KLid,27,0,2,4,1,      ! KOP(3) = 4 is Stiffness, = 5 is damping, = 2 is inertia output result
r,KLid,4725.1761,3258.2165,0,-33261.2676,1626946.9728,0,
rmore,0,0,0,0,0,0,
rmore,-3258.2191,4725.1777,0,-1626946.5781,-33261.299,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,-15434.1567,89265.2558,0,-5182223.0717,625042.0062,0,
rmore,0,0,0,0,0,0,
rmore,-89265.2446,-15434.1487,0,-625040.2455,-5182222.0351,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,
rmore,0,0,0,0,0,0,

mat,KLid
real,KLid
type,KLid
secnum,KLid  ! section ID
MP,BETD,KLid,0.00000001,0,0,0,0
EN,KLid,NodeJ,EPKL       ! define an element by the nodal connectivity

/SOLU

It appears that the snippet successfully created the MATRIX27 element. When I set:

ET,KLid,27,0,0,2,1,

to model the mass matrix of the bearing, I can see that the mass summary in the Mechanical Solution Information has really changed (Type 68945 is the MATRIX27 element type):

***********  PRECISE MASS SUMMARY  ***********

   TOTAL RIGID BODY MASS MATRIX ABOUT ORIGIN
               Translational mass               |   Coupled translational/rotational mass
        0.10000E+06    0.0000        0.0000     |     0.0000       0.44899E-02   0.47978E-13
         0.0000       0.10000E+06    0.0000     |   -0.44899E-02    0.0000       0.86666E-13
         0.0000        0.0000       0.10000E+06 |   -0.47978E-13  -0.86666E-13    0.0000   
     ------------------------------------------ | ------------------------------------------
                                                |         Rotational mass (inertia)
                                                |    0.18592      -0.25673E-11  -0.59732E-11
                                                |   -0.25673E-11   0.18592       0.46053E-11
                                                |   -0.59732E-11   0.46053E-11   0.94659E-02

   TOTAL MASS = 0.10000E+06
     The mass principal axes coincide with the global Cartesian axes

   CENTER OF MASS (X,Y,Z)=   0.86666E-18  -0.47978E-18   0.44899E-07

   TOTAL INERTIA ABOUT CENTER OF MASS
        0.18592      -0.25673E-11  -0.59732E-11
       -0.25673E-11   0.18592       0.46053E-11
       -0.59732E-11   0.46053E-11   0.94659E-02
     The inertia principal axes coincide with the global Cartesian axes


  *** MASS SUMMARY BY ELEMENT TYPE ***

  TYPE      MASS
     1  0.169594E-03
 68945   100000.   

 

 

However, the modal analysis results are the same compared to the results without the MATRIX27 element. Theoretically, if I create a MATRIX27 element with a stiffness matrix, the eigenfrequencies should be higher for the geometry that is radially and axially fixed on one side and founded with the bearing on the other side, and if I create a MATRIX27 element with a mass matrix, the eigenfrequencies should be lower. But no matter how I change the type of matrix or the values in the matrix. The results are always the same.

 

I also tried using the APDL command snippet object to create a generic joint, similar to the code I posted above. It works fine and gives the desired results. So I think it's because of my lack of understanding of the MATRIX27 element, even though I have read the element reference of MATRIX27 carefully. Could you give me some advice about this element? Thanks in advance.

Best regards,

 

Oliver

[dlooman]

MATRIX27 was used in the past for this purpose, but the introduction of element COMBI214 around 2010 made it unnecessary.  COMBI214 is a bearing element with a 2x2 stiffness and damping matrix.  The matrices can be unsymmetric and have negative off diagonal values (like for a journal bearing.)  Could you see if COMBI214 can model your bearing?

[OliverK]

Hi Dave,

Thanks for your reply. COMBI214 is unfortunately not enough to model the bearing, because it needs 4X4 unsymmetrical stiffness and damping matrices with negative values for the bearing in UX, UY, ROTX, ROTY directions. I just figured out why the snippet I posted above didn't work as I wanted, because I was attaching the MATRIX27 elements with pilot nodes that are fixed. I modified my mesh and created some nodes as fixed to the ground and attached the MATRIX27 elements to these nodes instead of the pilot nodes. After that it works fine. But now I have another question. While I was entering unsymmetrical stiffness and damping matrix with negative values using MATRIX27, ANSYS reminded me:

"For element type= (MATRIX27),KEYOPT(1) cannot be 1 when KEYOPT(2) is greater than zero."

Does this mean that I cannot enter a negative definite matrix if I set KEYOPT(2) = 1 (unsymmetric matrix)? For example, one of the stiffness matrices looks like this:

   1.0e+06 *

 

|    0.0047    0.0021   -0.0213    1.6272    |

|   -0.0021    0.0047   -1.6272   -0.0213    |

|   -0.0098    0.0891   -5.2080    0.3970    |

|   -0.0891   -0.0098   -0.3970   -5.2080    | ,

I applied the Cholesky factorization and found that this stiffness matrix is not positive definite. And I can see from the solution information that this matrix was not added to the model. But for the other damping matrix, which is positive definite, it was added. So will Mechanical just ignore the non-positive definite matrices and run the simulation without them? Is it possible to enter a non-positive definite matrix?

Best regards,

Oliver

[dlooman]

It seems pretty clear you can't use matrix27 to input a non-symmetric non-positive definite matrix.  My guess is the solver will stop or error out if you do.  I'm pretty familiar with rotordynamic analysis and I haven't ever encountered a need to do this.  What physics are you modeling that are so unique?