ANSYS prestress (stifness matrix extraction)

[mangelicamayorca]

Hello hello,

I am working in ANSYS and I only to get the stiffness and mass matrices for further analysis. I have a disk, which a model as only a sector, and I do the static and the cyclic modal analysis.
I know that ANSYS when solving for cyclic, doubles the matrices (double sector and basic sector) but when I extract the K matrix I only need the basic sector information, not both.

Do you have any idea of how I can get only the information of the stiffness matrices after prestressing of only one sector?

Thank you very much!!!

/Maria

 

[ansysfreak]

Hi Maria

Did you try the Cyclic,unbouble command?

Garry

 

[mangelicamayorca]

Hej Garry,
Well, I have actually tried. But in I am not sure if I have tried in the right stage. The procedure for the prestress is the following:
1)With only on sector of the geometry, create a cyclic static prestress analysis
2)Step 1) creates an .EMAT file that it needs for the modal analysis. I guess that I need to start the MODAL analysis in order to create the new stifness matrices. I need the files .full obtain the information, and this only done after starting to SOLVE.


The question is that if I undouble after the static analysis, the emat file is created with cyclic condition, and when starting the next calcuation (modal) to build the matrices, it has the information from this .emat file.
If I undouble after solving, nothing happens with already generated matrices. I hope I explain myself.

I am only interested in the stiffness matrices that includes the prestress, but not the double sector matrix.


Any other Idea?

 

[cbrn]

Hi,
I'm not so sure I correctly understand your procedure. However, here is what I usually follow in these cases. Note that the prestressed modal analysis can be cyclic or not, Ansys will handle it by itself, provided that the ciclicity is enforced using the "complete" CYCLIC,..." command and not a "simple" Coupled-pair method using "CPCYC,...".
1- in /prep7, setup your analysis as usual
2- in /solu, choose the static analysis type and BE CAREFUL to check the option "calculate prestress" in the analysis options
3- solve for the static part
4- re-enter /solu, i.e. choose now a "modal" analysis type. Take care to control that the options are those you need (right now I don't remember if there is again a checkbox with "use prestressed state" or something like that
5- solve for the modal part.

Note that with that procedure, the final result file will only be "modal-type", because the structural (prestress) results are overwritten in step 5 by the modal ones. If you have necessity to save the static solve results, simply make a copy of the ".rst" file after step 3 (or 4).

Regards

 

[mangelicamayorca]

Thanks!

Yes, I was doing the same procedure than you, but I was using CYCLIC command. When I use CYCLIC, ANSYS needs to create another sector for the analysis and this is what I didnt want.

So now I am trying to solve for only one sector, but using CPCYC it seems to work. I have to see what are the real differences in the prestress using CPCYC and CYCLIC in the prestress.

Thanks a lot!!

/Maria

 

[cbrn]

Hi,
there will be absolutely no difference in the prestress state, using simple coupled-pairs with CPCYC or using completely different cyclic formulation with CYCLIC.
However, with CPCYC you only enforce DOF equalities at the "lower" and "upper" end of the sector; that means that your cyclic model won't be able to determine eigenmodes which have a period which is not a direct multiple of the sector amplitude (i.e. which are not strictly cyclic-SYMMETRIC on their own). In other terms, if you had to analyze a turbine with 15 blades, a cyclic sector could encomprize only one blade (360/15° sector amplitude), but with CPCYC in the modal analysis you would completely "miss" modeshapes like the "bell" one, just to make an example. Instead, by using CYCLIC and its "Fourier-like" formulation of the loads, the restraints and the responses, ALL modes would be correctly reproduced.
So, be very careful following what you really need to do... Generally speaking, the modal (more in general: vibrational) analysis on one cyclic sector CAN NOT be generalized to the complete structure, UNLESS YOU USE "CYCLIC".
If still you want to get rid of the doubled sector, I believe there must be something you can do in Post-Processing phase. The idea of manipulating the matrices files directly doesn't seem a good idea because I think the rows are mixed-up by reordering right after the SOLVE command, in order to maximize efficiency (otherwise the only thing you would have to do would be to delete the rows/columns referring to the doubled-sector's elements. In order to know at which number they begin, first of all "compress numbers" of the original model before cycling it, then *GET the max elem number, then CYCLIC the model, etc etc; the first "doubled" element will have a number equal to "MAX-ORIG-NUM"+1).
Regards

 

[Zachary07]

I am interested in this problem too,
thanks all