time history analysis 1

[Buzzbromp]

I have a 3D model that is fixed at its base. I have both a acceleration time history and displacement time history to read into my model. I've tried 3 scenarios. First, i ran the acceleration time history on my model using using the mode superposition method. I applied the acceleration to the entire structure rather than just the base. I then did the same thing but instead of using the mode superposition method i used the full method. After post processing and finding for instance the time where i have my maximum moment at the base and comparing the two methods, i am finding that the mode superposition is giving me a moment approximately 50% greater than that of the full method. I was very surprised by these results and am wondering if there may be a reason other than my own algorithm.

Next i tried running the displacement time history at my base (which is also the location of my only boundary coundition, fixed). After plotting my forces along the height of my structure, it seems that my forces have a smooth transition from top to bottom until about 20% of the height from the bottom. At this point, the moments and shears tend to increase drastically, than jump around from say 800,000 to 30,000 within the next meter. I believe i should be able to apply the displacement time history to my base and this would yield the most realistic results, but I am wondering why my results seem to be so spuradic. Has anyone had similar issues? My next step is to try running the acceleration time history at the base only, but again, i'm not sure if that is something the program will let me do, since that is a fixed boundary.

I am using version 11.0. Also maybe of note, when applying the displacement time history, i essentially read my text file into an array, defined the rows to coincide with the time, and then applied a do loop that applied the displacements in 3 directions, i.e. d,selected base nodes,ux,temp_dispx; d,selected base nodes,uy,temp_dispy; d,selected base nodes,uz,temp_dispz. Perhaps since this is overwriting my original fixed BC of those nodes, it is causing issues?

Thanks

 

[cbrn]

Hi,
I see a severe issue in your applying the acceleration to the entire structure. It's not realistic: earthquake transmits to the structure only through the points which connect the structure to the ground; even if you are not dealing with earthquake, I see no mean of accelerating an entire structure in a transient way, except electro-magnetic fields or so.
For the mathematical consequences of applying acceleration to the entire structure, theory of multi-degree-of-freedom vibrations in matrix form is involved. Basically, you are cancelling out the contribution of modes whose shape "goes through" the structure, and you are only keeping the global acceleration stresses ("harmonic 0") and some harmonics excited by the self-displacements of the structure (i.e. internal strains).
There should be no difference (apart rounding errors) between applying a displacement time-history, a velocity time-history, and an acceleration time-history, because they are, in cascade, one the derivation of the other. ...Provided that, of course, they are applied in the exact same way. If you first involve the entire structure, and then only the base nodes, you are comparing potatoes with carots.

Regards

 

[Buzzbromp]

Thank you for your reply. Maybe i wasn't clear.

I understand that forcing the entire structure to accelerate due to the time history is not realistic. That is why I was trying to apply the displacement time history to the base. However, results do not look good as they shears and moments do not have a smooth transition through the structure. I was wondering if I am not able to model a displacement time history at the base because that is my original fixed BC. I also tried to use the cmaccel command on the bottom element (element attached to the base), however since that had one node fixed, its stiffness limited my response in the structure. I am now going to try to do the same thing, except remove my fixed BC at the base. Hopefully that will work, but i am thinking i will have issues because of no BC.

That was my main question, how do you typically apply a time history to say a cantilevered beam at its point of fixation? I know response spectram analyses have the response applied to the BC's, but I am not sure that time history transient analyses can do that.

My other question was why would my results from applying the acceleration time history using the full method be so different from that using the mode superposition method. I would assume my results would be different, but not to the percentage i previously mentioned.

 

[Transient1]

Hi,

I believe you should be able to apply your time history to a fixed support. Check the structural manual for ANSYS, it may be you can apply acceleration but not displacement (or vice versa). I know you can apply a random vibration (PSD) to fixed supports.

If you do not have smooth shears and moments, consider how you are connecting the different bodies of your structure. Are you using contact elements? Perhaps, you forgot a contact. I think its generally good practice that for any transient type simulation that you run a modal analysis with no fixed supports, unconnected pieces of your structure will stand out for each of the unsupported modes.

 

[cbrn]

Hi,
1- if you can't use a frequency-domain analysis (PSD excitation, response spectrum analysis), then I presume you have some non-linearity in the model. As Transient1 says, if the response is not "smooth" then either you have a connectivity problem (launch a simple eigenvalue analysis and see if you get some rigid-body motions or "half-structure" vibrations where two parts of the structure get "disconnected"), or a contact is missing (or is deactivated). When you have intermittent contacts, be sure to have "update at each equilibrium iteration" activated. Be careful when you use the "eigenmodes" check: if there is a contact, its status will be linearized i.e. the contact stiffness will be evaluated once at the beginning and then never updated, so if it's closed then the behaviour will be "bonded-like" regardless of the real kind of contact you have built.
2- applying time-history displacement is very easy even with the GUI, once you have prepared a TABLE for it. Instead, velocity or acceleration at restraints is not accessible via the GUI, you must use the "D" command explicitly (once again, the TABLE for the time-history must exist)
3- spectrum analysis and transient response are two completely different things and of course can not be mixed together. They belong to two different domains (frequency vs. time) and, moreover, spectrum response is:
- linearized
- steady-state (i.e. it represents the stabilized response of the system to an excitation composed by a "mix" of harmonics as in the spectrum which you define).
This is to say that, if the transient part of the response is "too long" and your TIME of transient analysis "too short", you won't be able to compare any result between the spectrum analysis and the transient one.
If you have troubles because the timeframe you need is very long, resulting in an enormous number of timesteps, then you can run a first TRANS to solve the "really transient" part, then save the results as initial state for a successive TRANS dedicated to the "steady-state" response. This will be the only way to analyze a non-linear structure.

Regards