Modal analysis with contact interaction

[Khal92]

Dear Abaqus users,

I need to perform a modal analysis of a compressor stator blade in an industrial gas turbine. The context of my analysis is the effect of fouling and corrosion in the blade attachment on vibration characteristics of the whole blade. In order to do so, I would like to take into account the contact at the attachment in my frequency analysis on Abaqus. I know that contact, which is non-linear, is ignored in modal analysis because it is linear. But basically I want to simulate the difference between a clean attachment with a clearance and a dirty one where some contact areas are steel-steel and other are steel-dirt-steel by changing the stiffness of the contact. For the clean one, because of the clearance the contact will vary depending on the mode shape (because it is a stator, no centrifugal force). For the dirty one, I will consider that the fouling clamps the root, thus the contact will remain the same with different contact stiffness along the root. I tried to simulate it by an elastic foundation but the clearance cannot be represented, that is why I ask you if you know a way to simulate this contact on Abaqus in order to find the natural frequencies of the blade, please. I read in a forum that performing a transient analysis will take into account the contact and applying an FFT on the response will give us the natural frequencies, so I tried the step modal dynamic but the contact interaction was ignored. I have attached the picture of a simple model of the attachment between the stator blade root and the outer ring (annulus) with an exaggerated clearance.

http://files.engineering.com/getfil...74-47990131883c&file=Blade_root+clearance.png

Thank you,
Khalid

 

[ebdoep2]

To be honest this is outside my wheel house, but no one else was taking a crack at it.

Would it not be possible to partition a small washer like region at the contact area which is tied (perfect tie constraint not a contact constraint) to both surfaces. Then by adjusting the modulus of this "washer" you can affect different boundary conditions. As the modulus approaches that of the original material (steel) you have a perfect connection. As the modulus approaches zero you have a loose connection/contact/interaction. This would eliminate the nonlinear issue of using actual contact conditions. While maybe not the perfect solution, it should provide some insight into how much of an effect this connection has on the structure.

Also I was not able to view your attached image just took me to a blank page.

 

[Khal92]

Thank you for your answer. I have already tried to do so but the problem of this simulation is that it introduce a tension stiffness into the system which does not exist. Basically, the contact stiffness is only a compression one (and also tangential normally due to friction but not taken into account for now).
I have attached the picture in a different format.

http://files.engineering.com/getfil...103-b26f-4cbe69fd0629&file=Forum_picture.pptx

What I am thinking to do is to perform a dynamic analysis of the system, which will include the contact, on which an impulse of force (like a hammer tap) will be applied so the displacement response signal will give me the natural frequency after an FFT (as in a basic hammer test). But I don't know which step should I use. I tried with a Dynamic, Implicit but I've got the following error message:
"Error in job Job-5: Too many increments needed to complete the step
Error in job Job-5: THE ANALYSIS HAS BEEN TERMINATED DUE TO PREVIOUS ERRORS. ALL OUTPUT REQUESTS HAVE BEEN WRITTEN FOR THE LAST CONVERGED INCREMENT."
So if anyone has an idea help me, please.

Thank you.

 

[dtm044d]

I did this awhile back using *Dynamic, Implicit as well. That is a good approach to capturing frequency response of a system with preload. If it's not solving due to issues with contact convergence, that is a separate issue. It sounds like the nature of your problem (varying clearances, opening / closing of surface contacts ) may be difficult to solve using contact in general. The first thing I would do is use tie instead of contact - always nice to do to get your analysis process set up with simple/rigid contstraints. I would even record a value for first natural frequency to use later for comparison to runs with varying degrees of contact. Once you get that, move to a clamping condition that represents full contact / max preload, something that ensures a large amount of clamping contact in the step prior to your *Dynamic, Implicit step (akin to a bolt clamping preload step). I would even use a high degree of friction even if its unrealistic. Once you get something to solve, you can move from there to vary the parameters of contact that represent the different conditions you need to simulate.

For what its worth, I have also performed this "hammer test" using *Dynamic, Explicit. I gave an initial velocity to a rigid block (hammer) and allowed it to contact a plate. Then I used an FFT Abaqus plugin to post process the history output of acceleration near impact. My plate was hanging off a string (connector) with only gravity acting prior to impact. I imagine you could apply your preload in a previous step and then whack it with a virtual hammer. Sometimes jumping to explicit with complex contact conditions can be nice, but post processing is more difficult (and analysis can be less accurate if you don't know what you're doing).