In the sequential wind coupling method, the aeroelastic analysis is performed by the aeroelastic code with the effects of the supporting structure incorporated as a superelement to the solution. Mechanical APDL provides the supporting structure substructure matrices and loading data that are required as input to the aeroelastic code. After the aeroelastic analysis, the results can be fed back to Mechanical APDL to recover the element forces inside the supporting structure.
The procedure for carrying out an integrated wind and wave load analysis is described as follows:
The wind turbine supporting structure is modelled in Mechanical APDL. A substructure model is created with the top node (i.e. the connection point between the wind turbine and the supporting structure) set as the master node. This master node must have 6 freedoms: UX, UY, UZ, ROTX, ROTY, and ROTZ. A substructure generation run is performed with the supporting structure model subjected to ocean wave and other external loadings. The solution times for this run should tie in with the times of the solution that will be attempted in the following aeroelastic run.
The command OUTAERO can be called after the solution from 1 is obtained to produce the generalized mass, damping, and stiffness matrices of the supporting structure, together with a time series of the generalized foundation external loading (due to wave loading etc.). The generalized matrices are written to 3 separate files (mass, damping, and stiffness) and the generalized load time series is written to another file. See Output from the OUTAERO Command.
An aeroelastic solution is then carried out with the foundation effects included through utilizing the generalized matrices and loading vector derived above. The forces and/or displacements at the supporting structure top node at each solution time are written to a file.
Another Mechanical APDL run is performed to recover the member forces in the foundation structure by applying the supporting structure top node force or displacement time series obtained from the aeroelastic analysis together with the foundation external loading as specified in step 1. The analysis can be carried out statically or dynamically.
Note: The following points should be noted for the sequential solution approach:
The generalized matrices (stiffness, etc.) are computed based on the initial undeformed geometry and assuming small displacement, linear behavior. It is thus implicitly assumed that the foundation is linear with small deformations throughout the entire solution.
Likewise, when computing the generalized foundation external load time history in the substructure generation pass, it is assumed that the structural displacement and velocity are zero since such information is not available when the loading is generated.
The hydrodynamic mass for the supporting structure is formed based on the water elevation at the first time at which the solution is attempted.
If the supporting structure internal forces are recovered statically in step 4, the dynamic forces (e.g. inertial force) in the foundation will be ignored. The dynamic effects can be accounted for by running this step as a transient job. However, it should be noted that the following points may affect the accuracy of the solution:
The generalized mass used in the aeroelastic analysis is only an approximation to the true mass matrix (static reduction is exact but not dynamic).
Different time integration schemes may be adopted by aeroelastic code and Mechanical APDL. Hence, while the displacement time histories are identical in both runs (for the prescribed displacement case), it may not be the case for the velocity and acceleration time histories.
There should be little difference between applying forces or displacements to recover the foundation forces. The two methods should yield identical results in a linear static analysis.
This approach should be much more efficient than the fully coupled approach as there is no need to keep both the aeroelastic code and Mechanical APDL running simultaneously and keep exchanging information every time step.
Four formatted ASCII files will be generated by specifying the OUTAERO command macro. These are:
Jobname.gnm - generalized mass
matrix file
Jobname.gnc - generalized damping
matrix file
Jobname.gnk - generalized
stiffness matrix file
Jobname.gnf - generalized external
force time series file
where Jobname is the current job name.
The generalized mass, damping, and stiffness matrices are formed based on the information at the very first load step and are written to 3 separate files. These are formatted ASCII files with the full 6 x 6 matrix included. The files are written with the following format:
ngenfr (1x, I6) (val(i,1), i = 1,ngenfr) (6(1x, E12.5)) (val(i,2), i = 1,ngenfr) (6(1x, E12.5)) . . (val(i,ngenfr), i = 1,ngenfr) (6(1x, E12.5))
where ngenfr is the number of generalized freedoms,
which is always 6 at present, and val is the generalized
matrix.
The row and column order in the generalized matrix corresponds to the order UX, UY, UZ, ROTX, ROTY, ROTZ.
A time series of the generalized foundation external loading vector is written to another file. At each solution time, the time (t) and the associated generalized load vector (f) will be output to this file. The force file has the following format:
ngenfr (1x, I6) t1 (1x, E12.5) (f1(i), i = 1,ngenfr) (6(1x, E12.5)) t2 (1x, E12.5) (f2(i), i = 1,ngenfr) (6(1x, E12.5)) . . tn (1x, E12.5) (fn(i), i = 1,ngenfr) (6(1x, E12.5))
The load values are ordered in the same way as the generalized matrices.
This is an example of the sequential aeroelastic analysis process. This first analysis is run to create the matrices/loading. These are generated by the OUTAERO macro near the end of the analysis.
The master node is set as node 9, which will be the interface point to the aeroelastic structure.
/verify,airysublarge /FILNAME,airysublarge /prep7 /TITLE,airysublarge, WAVE ON MONOPILE /com ************************************************************************** /com Substructure with Airy wave /com use time to determine phase at each step /com includes current /com CREATED 08/03/11 /com ************************************************************************** antype,substr seopt,monopile,3,1 nlgeom,off et,1,pipe288 keyopt,1,3,3 keyopt,1,12,1 type,1 mat,1 ! Define pipe section secnum,1 sectype,1,pipe secdata,1.0,0.1 ! Define ocean matwat=2 idwat=2 idcur=3 idwav=4 depth=30.0 offset = 1.5 ! Ocean basic octype,basic,ocean1 ocdata,depth,matwat octable,,,0.7,0.7,,2.0 mp,dens,matwat,1000.0 ! Ocean current octype,curr octable,0.0,1.0 octable,-depth,0.0 ! Define geometry of vertical tube n, 1, offset, 0.0, -30.0000 n, 2, offset, 0.0, -25.0000 n, 3, offset, 0.0, -20.0000 n, 4, offset, 0.0, -15.0000 n, 5, offset, 0.0, -10.0000 n, 6, offset, 0.0, -5.0000 n, 7, offset, 0.0, 0.0000 n, 8, offset, 0.0, 5.0000 n, 9, offset, 0.0, 10.0000 n, 900, offset, -20.0000, 0.0000 en, 1, 1, 3, 900 en, 3, 3, 5, 900 en, 5, 5, 7, 900 en, 7, 7, 9, 900 MP,EX, 1,2.0e11 MP,PRXY,1,0.3 MP,ALPX,1,0.0 MP,DENS,1,7850.0 ! Damping factors alphad,0.1 betad,0.01 ! Suppressions d,1,all ! Master freedoms m,9,all finish ! Increase limit of time values to 5000 /config,numsublv,5000 /SOLU acel,0,0,9.81 wper=10.0 phs=0.0 ! Ocean wave (Airy in this case) octype,wave ocdata,0,0.0,0,1,1 octable,2.0,wper,phs tm_1=1.0e-8 tm_2=1000.0 tm_inc=0.2 *do,tm,tm_1,tm_2,tm_inc time,tm solve *enddo ! Print substructure matrices ! outaero,'monopile',tm_1,tm_inc ! This version uses the time defined by tm_1 & tm_inc outaero,'monopile' ! This version reads the time off the .sub file finish
At this point the aeroelastic analysis can be run, using the output from the above analysis. Once complete, a second Mechanical APDL analysis is run with a time series of forces and/or displacements at the interface node. These need to be converted from the aeroelastic output to Mechanical APDL compatible output by the user (for example, using Excel) or the aeroelastic analysis program. Any ocean loading or extra loading included in the substructured analysis should also be applied in the subsequent analysis.