Just a few things to mention on your non linear simulation study which may point you in the right direction:
1. Just looking at the numerical data first, in the graph you plot you seem to be getting a fluctuation of between 8mm to 14mm (range of 6mm) for the resultant displacement (x, y and z directions). Small fluctuations in the three different directions as the numerical solver evaluates and re-evaluates the loading will cause the 'noisy' results. You may want to only plot resultant displacement in one particular direction (y deflection) to see a clearer picture of the true deflection in the direction you are interested in.
2. I took a quick measurement of the length of your longest beams where the node is located at the centre. These are modelled as 14,600 mm (14.6m) in length. Considering a worst case 6mm range in deflection results, this works out to be around 0.04% of the total beam length (6mm/14,600mm x 100) when experiencing a 26.180kN load. Which is well under 1% so such small variations are pretty much negligible and just due to the FEA model setup such as meshing and numerical rounding etc.
3. You are also capturing data in 0.1s increments over 10s so only have 100 data points which may not be sufficient in capturing the small changes over time skewing the true response at this point over a given amount of time. If you have the available time and processing power, try reducing the increments to 0.01 s and running for a smaller length of time (1-2 seconds) to test this.
4. You also have the large problem flag/solver in use for this study (try using auto or Intel Sparse in the study properties box), and have no damping at all in this system to smooth out the response so it may be worth checking if any damping exists in this system.
Some of those tips might help!
Assuming I looked at things correctly as I did not down load the model, your load curve appears to have the load being instantaneously applied at t=0 so the vibration should be expected. No idea what your objective is here but if this was my problem I would first do a freqency analysisfor say 20 modes to know what sort of frequencies should be present in an NL dynamic analysis. Not sure why you are doing an NL dynamic as there does not appear to be any non linearities present. Deflections r small no contact.
Thank you very much to reply my question.
This model is a gantry structure. I need to study what kind of vibration occurs if it loss the lifted weigh suddenly.
Also i wish to run second study to study what happen to structure when apply sudden brakes to moving gantry.
Through those two studies i will decide applying requirement of ribs to this structure.
I have no clear idea how to do this. So first i started with NL dynamic because LD not available. gravity feature.
One time i tried to use LD by importing gravity deformation from linear static studdy. below i shown the used time curve and
I know something wrong what i'm doing. My gest was the time period 1to 2 second movement need linear.
But it show as vibration.
Could you please help me step by step which i need to follow to achieve my requirement.
The vibrations you see as others indicated due to the excitation of a natural frequency/mode, something that is normal and can be understood with a single degree of freedom (sdof) system where a suddenly applied constant force has bee applied to it. In such a case a transient vibrational motion follows (vibration), and with damping that will settle to a constant displacement due to a constant force.
If you do a modal analysis like suggested you will see that there is a mode close to 10 Hz, with motion in y-dir., which is what you call the unknown frequency/mode in one of you posts, so it is not unknown it is just a natural mode of vibration that is excited by the sudden force and that is and will be present in your results.
With 1 % critical damping (alpha=0.11, and beta=0.000289, for omega=1-10 rad/s) a fairly common assumption for steel structure, the system will oscillate in the first instance about the static deflection value for a static gravity and a static force (~ -11 mm), with an amplitude of about 8 mm, thus resulting in a largest y-dir. amplitude of -19 mm, just as seen in your image (https://forum.solidworks.com/servlet/JiveServlet/showImage/2-893770-440103/123.PNG ). This is quite consistent with sdof theory, where the largest displacement due to a sudden constant force is twice the static deflection (this is valid only for small damping or none).
As mentioned though with damping this oscillation will die off and if the force is held the displacement after some time will be that of the static solution, that is -11 mm.
Hope this explains to you, why you see the oscillation in your results (it is just normal).
Thank you very much to given valuable instruction.
As implied by Erik it would be a good idea to study up on 1DOF system behavior. You could try here: (Vibration - Wikipedia ). A few things to understand might be: a zero height impact has a deflection of 2x the static deflection. Imagine an elastic band with a weight on it. and your are holding the weight at the relaxed length of the elastic and then you let the weight drop. the peak deflection will 2x the static deflection once the oscillations stop. Damping sucks energy out of the system and typically generates some heat for material damping or causes the air around the structure to move and dissipate energy for viscous damping. Coulomb friction shows up in joints and does pretty much the same thing. So the general procedure is to get familiar will your structure by doing a frequency response to know what modes are going to be excited by your vibratory inputs. You generally want to have the mass participation factors in all 3 directions to be above 80% but this is not always possible, depending on the problem. The highest of the frequencies will determine your temporal resolution say 1/10 of the shortest period might be a good number in a dynamic analysis. the duration would be governed by the longest period and how much time you want to capture. If you have no non-linearities a good choice is linear dynamics. IF you have no clue on damping (as is often the case) a few percent for a logarithmic decrement is not a bad choice. Damping is usually determine in test or by experience (doing many similar problems and testing the response to develop a feel for your class of problems). The purpose of a dynamic analysis is to try and capture the dynamic amplifications due to the proximity of the excitation to a natural mode of vibration, attenuated by the damping. If no damping or insufficient damping is present and the vibratory input is on going then the structure will gain energy until catastrophic failure occurs. For a single event load input a dynamic analysis may not be necessary. A static analysis with some logic maybe sufficient to bound the response. Alternatively a short dynamic analysis that captures the peak of the initial response maybe sufficient (lowest order mode of interest). It really helps to understand the behavior of a single mass damper systems vibratory response to gain some insight into how structural dynamics behaves. It is much easier to help when some understanding of what you are into is conveyed in a question. If you have some understanding of the phenomena involved then running the program is much easier.
Thank you answer with nice example.
Pretty enough to understand the phenomenon.