Learning Forum

[omidrastkhiz]

Hi everyone,nI have a small question,nI am trying to model one segment which in reality I am conducting an experimental modal analysis (EMA),nbut I put the structure ( look likes Cubic) from it's four corner on top of the 4 springs, ndoes anyone know how I should define boundary condition related to the spring direction?nI mean should I use remote displacement, if yes, how?nThank you,nOmid.n

[omidrastkhiz]

Is it like normal boundary condition like normal free displacement boundary condition?

[peteroznewman]

Array nPlease insert an image (photograph or CAD geometry) of the complete structure and how it is supported for the EMA.nInsert another image showing the segment of the complete structure you wish to have an ANSYS model of.nWhat kind of analysis do you want to do on the segment? A modal analysis of a segment will not be useful in relation to the EMA on the complete structure.nWhat is possible is to idealized the complete structure, for example, to replace a compact subframe with an equivalent mass that connects to the same points on the structure.nPlease add details about the 4 springs.n

[omidrastkhiz]

This is 1/8 of the stator of the direct drive generator, nWe put the segment on 4 legs, ( which is actually a few spring in each leg in Z direction ), we also add a shaker with sound underneath which is not relevant for now,nMy question is how to model the boundary condition for this structure? in X and Y direction we fixed with 4 brackets it which means there is no displacement in this two direction for each leg, I did not draw it brackets here, nI can set no displacement for X and Y direction around for legs but How I define boundary condition in z direction because of spring?.Thank you so much for the response and Happy New Yearn

[peteroznewman]

ArraynI misunderstood your meaning of a segment. A segment is the name of the part you are testing. Eight segments are assembled to make a complete stator, but you are not testing the complete stator, you are testing a segment part on its own.nThe brackets on each corner that control X and Y should be added to the simulation as they will interact with the segment to constrain motion in those directions.nThe bracket design is important. If you hold four corners of a part fixed in X and Y, that is 8 constraints, which is an overconstraint since there are only 6 DOF for a rigid body and at least one DOF, Z, you want to be free to find equilibrium with the springs.nPlease provide details on the corner brackets.n

[omidrastkhiz]

nThanks a lot for the resoponse,nIs there any chance that I can send you an email? since some of the pictures and details are confidential, I am not sure if I can put them here, so if it is possible please send me an email : S181334@student.dtu.dk, in this case I can explain better, sorry for asking this, Thank you so much, nBy the way, you understand what I meant completely right, and I can add zero displacement in X and Y direction for each corners instead of drawing geometry of the brackets in ANSYS, but I don't know what I should do in Z direction because of springs, I know it can move up and down and there is no limit for displacement, but it is a harmonic motion so I think it should has a customized boundary condition in Z direction (I am not sure If I am right or not for customizing Boundary Condition) , so I basically I mean, instead of setting the springs(drawing the real springs with their specific stiffness) in Spaceclaim, is it possible to set a boundary condition for it in Z direction?n

[peteroznewman]

nI have saved your email address. You might want to remove it from the post above if you still have time.nUnder the Connections folder, you should insert four springs to ground and orient them in the Z direction. You can enter the known spring rate. This will be a sufficient connection in the Z direction and you can add X and Y displacements on each of the four corners, though modeling the brackets would be better.n

[omidrastkhiz]

Hi Again,nThanks for the response, I did what you said, and here is the close example of what I did, my final goal is to find a natural frequency of the this segment ( which is close to this one), and for the real experiment, we have to suspend the structure with crane to simulate free-free boundary condition, but since it is heavy , due to safety reasons, we can't so, we need to put it in 4 (set of springs) to simulate free-free boundary condition ( meaning put it on very soft place) , and then with a shaker and accelerometer find natural frequency(Modal part in ANSYS) and FRF function (Harmonic Response in Ansys), ( displacement 1 to 4 is for No movement in X and Y direction for edges in four corners)nso here as you can see the first 6 modes are translation and rotation modes, which we can ignore, but do you think, this is a right set up for the whole experiment to find natural frequency of the segment and FRF function?nThe reason that I am asking for, is because for the 7 mode, it just shows the segment goes up and down on spring like because it's own weight and almost no shaking or vibration is shown, but my goal is to let it go to the equilibrium point and then use shaker or impact hammer, and for the 8 to 10 modes shapes it doesn't show any movement at all.nThank you so much, I really appreciate your help n

[peteroznewman]

nThat looks like a reasonable Free-Free model and it is correct that the first nonzero frequency mode is the mass pumping against the springs. You can calculate that frequency by hand since you know the mass and the spring rate using f = sqrt(k/m)/2pi.nIn a Modal analysis, there are no loads, so you don't have gravity deflecting the springs to a static offset, but in a Static analysis you do.nIn a physical experiment, the first six modes in the analysis won't be measured. Mode 7 in the analysis will be the first mode that can be measure by an accelerometer.n

[omidrastkhiz]

nI have been working on the model, and It seems it has almost the same natural frequency(NF) as I get from formulation as you said, which is for the third NF, and the seventh NF is start point for model and experiment to have compatible results, ( in case of only having spring in Y direction and no constraint in Z and X, which means I removed no displacement constraint), although I don't know why are the first six natural frequencies a nonzero result? nThose are 0 - 0 - 2.4 - 13.8 - 27.6 - 32.5(Hz) and the mass of the segment is 4250 and I used 4 spring with 252000 stiffness for each (in the formulation it should 4*K), and formulation result is 2.4 Hz.ndo you know what could be the explanation for these 6 nonzero results?nand do you know any book or any document for the explanation of mode shapes, which can help me to have a better understanding of the dynamic behavior results, like which one could be right and which one could be wrong.nThe 7th one starts from 57 Hz.n

[peteroznewman]

nWhen there are no springs to ground, the first six modes are the rigid body modes and the frequency would all be basically zero. Once you add four springs in the Z direction, you get one nonzero translation frequency in the Z direction and three nonzero rotational rigid body modes. You can see the part rotating. Mode 7 is the first bending mode of the segment.nRight or WrongnAll the nonzero modes in the model can be measured in an experiment with accelerometers. It is not a matter of right or wrong, it is a matter of accuracy. For example, the 2.4 Hz you calculated using the effective spring rate and mass might be measured in an experiment as 2.5 Hz. That means either the mass or the spring rate in the model needs to change. Given how easy it is to weigh the part, it is likely that the mass input to the model is correct, and the spring rate has to change. Once you look at mode 7, if that is off, then the stiffness of the part has to change, such as a wall thickness.nn

[omidrastkhiz]

nYes, you are right, once again thank you so much,nnAnd one more thing, now I am doing a harmonic response analysis, and in real case, harmonic force is applied to the segment with stinger ( like a narrow rod which is connected to harmonic force source), so if you imagine this stator segment as a curved plate with dimonsions 3*2 m^2 and thickness of 1 meter, made of steel which is stand on 4 springs, nI am applying 3000 N Harmonic force to the underneath corner of the segment ( weight of 4300 Kg), and 3 FRF diagrams of one node in X,Y,Z directions don't show all of natural frequency(NF) in the range of 0 to 420 Hz, which means in modal analysis, I asked for 16 NF and it starts from 0 to 420, but in FRF graph I can't see peaks for some of the NF?nsome of them are almost the same as the NF, could it be because of the frequency response point (the node I selected on the geometry), and also direction of the load ?( If you need the graphs please let me know)nand if I want coherence graph, I need at least to FRF graph I think, and do you know if it is possible in ANSYS?nmoreover, do you have any course that I can participate in or a channel for learning video in ANSYS? or do you know any link, pdf or any documentation that can help to have a better understanding of dynamic result for example for harmonic response result, mode shapes, phase diagram, coherence, etc ...,nThank you so much,nOmid.n

[Rajesh SBM]

I am doing a global FE Analysis for a mooring pontoon for different load conditions (deck load, wave load(hogging and sagging), other environment loads and etc,) in ANSYS APDL (static, structural). actually, the model floats in the water. Wanted to apply theoretical spring support ( resilient supports) at the corners that hold the model, in order to get stability in the model, and how to apply spring boundary conditions at the bottom of the model. Please kindly suggest. Element Type: SHELL181, Analysis: Static structural