Aeroelasticity (SOL144) - Problem with constraints

[JulienE]

Hi everyone,

I have a problem running my static aeroelastic analysis problem.

It consists of one wing represented as different beam elements along the span of the wing (has a kink).
To the nodes connecting the spanwise beams also always leave a beam towards the leading edge and one to the traling edge.

I have clamped the root (Node 201) with SPC1 1 1246 201.
And nodes 101 and 301, which are the leading and trailing edge at the root with SPC1 2 246 101 301.

Further I have specified a SUPORT 35 201 to perform the TRIM analysis.

I think this should sufficiently constrain the model. However I'm getting the following error.

*** SYSTEM INFORMATION MESSAGE 4159 (DFMSA)
     THE DECOMPOSITION OF KLL      YIELDS A MAXIMUM MATRIX-TO-FACTOR-DIAGONAL RATIO OF    8.627062E+07
 *** USER WARNING MESSAGE 4698 (DCMPD)
     STATISTICS FOR DECOMPOSITION OF MATRIX KLL.
     THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
     1.000000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.
     USER INFORMATION:
     THIS MESSAGE MAY BE IGNORED IF NO GRID POINT IDS OR HIGH RATIO MESSAGES APPEAR IN THE TABLE ON THE NEXT PAGE.
1    MSC.NASTRAN AEROELASTIC JOB CREATED ON 30-NOV-12 AT 18:31:27          DECEMBER   1, 2012  MD NASTRAN  12/15/10   PAGE     8
     UNTITLED.SC1                                                                                                                   
0                                                                                                            SUBCASE 1              
0                                                                                                                                   
         GRID POINT ID       DEGREE OF FREEDOM   MATRIX/FACTOR DIAGONAL RATIO        MATRIX DIAGONAL                                
                                                                                                                                    
             209                    T1                   2.32532E+07                   2.46890E+16
             212                    T1                   2.68200E+07                   2.46728E+16
             212                    T2                   8.62706E+07                   8.00587E+15
             214                    T1                   1.70589E+07                   2.46624E+16
             214                    T2                   2.53534E+07                   8.03312E+15
             217                    T1                   2.55754E+07                   2.46445E+16
             217                    T2                   5.81368E+07                   8.07818E+15
             220                    T1                   2.59770E+07                   2.46251E+16
             220                    T2                   5.01106E+07                   8.12882E+15
 *** USER INFORMATION MESSAGE 3035 (SOLVER)
                                  FOR DATA BLOCK   KLR     
    SUPPORT PT.NO.             EPSILON             STRAIN   ENERGY     EPSILONS LARGER THAN 0.001 ARE FLAGGED WITH ASTERISKS
                1          4.9240492E-14         -2.6321411E-04                 
                2          4.9240492E-14         -2.2796631E-02                 
 ^^^     
 ^^^ USER   FATAL   MESSAGE 9050 (SEKRRS)    
 ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. 
 ^^^ USER ACTION:  CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO                                
     CONTINUE THE RUN WITH MECHANISMS.

I have tried to run a modal analysis with the same structural model and this runs without problems. I'm guessing it goes wrong
somewhere in the definition of the splines. I'm currently using SPLINE4.

What I find weird is that nodes 209 - 220 are located from the kink to close to the wing tip, along the elastic axis.
Why is there a problem only at those nodes and not the others?

I will check tomorrow if I can perform a Flutter analysis with only one aerodynamic surface and spline defined and no elevator.

I have attached the .bdf and .f06. Hopefully somebody can give me a hint.

Thanks anyway!

 

[JulienE]

The .f06 ...

 

[nlgyro]

I guess the best bet is to package all your run file and contact the nastran tech support.

BTW, have you tried using param,maxratio,1.+8 on your input deck? MSC does recommend using maxratio in the order of 1.+7 to 1.+8 on most production models. I don't think the loss of one significant digit is going to affect your solution accuracy!

 

[JulienE]

Thank you very much for your response.

First of all, fortunately I've been able to solve it over the weekend.

I found several errors which may have caused the problem.
One is the fact that the research student of whom I got the model represented rigid beams as normal beams with a Younghs modulus of 10^20 GPa, I guess that the 10^10 order of magnitude with the other beams is not appreciated by the solver.

An other problem seemed to be the aerodynamic coordinate system which had the Z axis pointing upwards just as the reference coordinate system. This caused a negative angle of attack and negative pressures which didn't made sense.

Thanks for the proposal to contact MSC but from their site I found that only commercial customers can use the support.
However, they seem to have some support personnel on their forum.

Kind regards.