Help for Fixed plate resonance analysis.

[Allen110]

Greetings all
I am completely new to ANSYS, and I have a problem about my univercity project.I should analys the turbine end cover resonance whith ANSYS, and derive the three dimentional
mode shape. The end cover is like a square and fixed at the ends.the operating speed normaly varied between 3500 and 3750 RPM. and the thickness is 0.625 inch.and between bolts are 28.5 inch. and the plate lenght is 30 inch.

My question is that how should I apply the speeds mentioned above, and should I verify bolts in ANSYS like keypoints? And if any other help or sugestions you have, I will be glad. Thanks all.

 

[ISEAG]

Allen4

What you need to do is run a modal analysis of the plate with boundary conditions (temperature, ux,uy,uz). If I read your inquiry correct you don't need to apply a dynamic loading. You onbly need to run a dynamic loading to obtain dynamic stress levels. Plot your mode values on a Campbell diagram and you will see where the mode crossings at excitation levels of 1e, 2e, 3e, etc cross your modal results. You can then evaluate if the mode shapes correspond to the particular crossings on the diagram. I have completed this exercise countless times on several turbine engine static components. The hardest part is learning to identify the nodal diameter count of a particular mode shape. Good Luck.

 

[ISEAG]

Allen

Sorry, forgot to answer part 2 of your question. I would fix the 3 translations at the bolt locations for a simple solution. Reality of the situation is that it isn't cost effective to model the fastening with anything more than a point load. It is often reasonable to couple all of the nodes in the plane of the flange so that it remains plane. Some will argue that you miss the out of plane motion of the plate between bolts but I have yet to see a vibration failure due to this mode. It depends on who the engine company is but for a university adventure such as yours, it might be fun to impress your prof with the notion that you thought of this possible constraint. Try it with and without the coupling just to see the difference in the results. For the low engine speeds you are concerned with, you probably won't see this response as a concern.

 

[Allen110]

ISEAG
Thanks alot for you explanations.
You said that you had experiences about this, do you have your sample .db files about this? I mean is it possible to send me, then I can check mine with yours and optimizing my design.
Thanks again.

 

[ISEAG]

Allen

Sorry to disappoint you but the model files I have produced over the years are the property of and in the possession of the engine companies I have worked with.

If I get some time later today, I wll try and get you a small model set up for this type of anlaysis. IT is quite simple. Just build your model and set the solution for a modal anlaysis using Bloc Lancos solver. Request 20 extracted modes and a frequency range of .001 to 4000 Hz. I believe you will find that your plate is quite stiff and the first mode will be well above a 4/rev (also known as 4E)excitation at 4000 RPM. Depending on blade count and mass, most turbines don't have an excitation level above 4E that will effect a plate such as this........and if it does, it will be low energy and won't be a problem any way.

Glen

 

[Allen110]

OK, Thanks again , I've done my solution perfectly, now there is only one problem for my last step and it is:
Now I should derive the 3D mode shape plot while the plate is experencing  15200 CPM frequency.I have done the solution but I have trubble deriving the 3d plot which must
be an x,y,z axis and for example the x and y should be the two sides of the plate and z must be the amplitude.
How should I get the plot?
Thanks

 

[ISEAG]

Allen

Sorry for the delay. I got sidetracked over the last week and lost track of this thread. Hopefully you found your answer. If not, what I think you are looking for is a displaced mode shape plot. Your desired frequency is at 15200 cpm whicj corresponds to 253.3 Hz. Your Modal solution output is in Hz (cps). Chances are you won't have an eigenvalue at your desired frequency so you look at the mode shapes above and below your desired set point. The idea is to have a margin in frequency above and below your set point (253 Hz) so that you will not have a resonance. The best I can tell you about the actual "mode" shape of your part at your desired speed is that it will be displaced somewhere between the eigenvalue above and below your desired speed. I have not done straight up dynamic loading on parts...........a dynamicist I am not........so I am not sure how to apply an exact frequency and extract the displaced shape. Never really wanted to for a static component such as a plate. Out here in the non-academic world we don't concern ourselves with what something looks like when it doesn't fall into a problem area..........

For example, your plate would be deemed okie-dokie if the operating frequency (253 HZ)was at least 15% away from the part's nearest modal solution eigenvalue......so as long as the shapes are below about 220HZ or above 285 Hz we would say it is ok.

Sorry I couldn't give you the straigh skinny on this one.

Glen

 

[br33zala]

hello glen,
Is it possible for you give the input listing of any solved problem.I would appreciate if you can give that.
regrads,
ZALA B
email:bzala@hotmail.com