A change in stiffness may not be an obvious deformation.
A classic example is a guitar string; w/out the prestress the modal will not show the correct freq (note), but the shape doesn’t change in statics is a tensile load, same with prestressing long bolts, they can change the modes but the don’t even need to bend to do that.
A microphone diaphragm is the same, shape remains, [K] matrix changes.
1 Like
Welll,…I don’t completely agree.
You need the deformed mesh to correctly reconstruct the mode shape.
I think the perturbation is doing it correctly and we are both right .I think this is just a visualization problem in which Prepomax is applying the results (displacements) to the original mesh instead of the deformed one.
I don’t know which could be the motivation behind other programs when using the original mesh but according to what FeaAnalyst has post Abaqus would be building the modeshape from the deformed mesh as base.
Can’t be. what units/amplitude of disps do you use then since modal has no loads?
In linear dynamics all it matters in the modal is the K/M ratio, since K is adjusted from static preload, job done, the maths cannot do anything else on a modal analysis; like a guitar string.
I don’t debate that someone, somewhere may have implemented a normalised static super-position somehow; but you are faced then with another problem, what ‘phase’ do you use for the deformed shape; i.e. what is positive and negative on peak disp areas.
A modal analysis doesn’t know that, one side is opposite the other peak in disps and it stops there till you do a forced response with actual loadings.
Just seen this proper in your post:
I see where the confusion is coming from, it should be the stiffness, not the absolute results from statics that the modal reuses. Sorry, I should have read posts better.
It is the [K] matrix change all you can do for a linear modal.
1 Like
sentences in manual cannot be improperly in use since all stressed structure also deformed, but probably it changes the stiffness due to stress not based on geometry after deformation.
since it’s related to previous stress not deformation, a plot of CalculiX or PrePoMax more relevant than Abaqus.
This is just the Frequency analysis results visualization. No dynamics yet. I understand amplitudes of the displacements (and stresses) are scaled and don’t correlate with real world but ¿how do we build the eigen-shape?.
TKosir is surprised that “mode shapes oscillating around undeformed shape”. That’s what is also weird to me. Looks like mode shape to display on the screen has been built like “initial mesh + displacements results from STEP 2" rather than “deformed + displacements results from STEP 2".
For the analisys I agree.
To prepare the visualization of the results you also need a mesh where to apply the displacements?. Which one is the right one to use, the initial or the deformed from step 1.?
this can be the proper in modeling, i can confirm by compared of eigenbuckling with perturbation and imported deformed mesh shown large discrepancy in factors, stress distribution also.
What about the stresses in the model (pre-stress). Do you also transfer them?
Example.
1-Linear static compression of a vertical beam
2-The beam becomes shorter.
3-You transfer the new geometry
4-Perform a Linear buckling analisys to the new geometry
???
Doesn’t have sense to me .The buckling load will be wrong if you don’t transfer the stress state in the beam to the new buckling step.
when needed both of stress and deformation effect to consider, still imported deformed mesh is proper ways in modeling. Stress stiffening or softening can be included by initial condition, it seems perturbation only appropriates for case of deformation is small and insignificant.
even the manual documentation notified both are considered, but it’s not good choices to fully trusted without any testing and verify.
It’s a silly example, but it illustrates the problem.
Imagine you want to calculate the vibration modes of an erected tent.
You take your tent, spread it on the ground, take your tent poles, apply force and bend them. Then you fix them toghether and to the ground so they don’t move (END of STEP1).
Now I’m going to calculate how my assembled tent vibrates.
You tell the solver to do a Frequency analysis with peturbation taking into account the deformations and stresses in the tent.
“By using the parameter PERTURBATION on the *STEP keyword card the user specifies that the deformation and stress from the previous static step should be taken
into account in the subsequent frequency calculation.”
When I look at the solution, one would expects to see oscillations of something tent-shaped not oscillations of of something like a tent flat on the ground.
I don’t know if I that helps?
1 Like
Good pic, but that is a highly non-linear FEA, the geometry changes completely from ‘flat’ to erected.
That already breaks what a linear system, like a modal analysis can do.
The tent should be modelled erected from CAD ==> pretens axial stress/forces on rods ==> pass onto modal analysis via [K] matrix change ==> get the correct (assembled tent) modes.
I think we are mixing things up here: what something does in real life, like the tent from flat to up; and what a linear system like a modal solve can do.
Think of the guitar string case, the geometry doesn’t change when tuning up (static preload), then same ‘initial’ mesh + [K] matrix add from statics gives you the correct LINEAR modes.
If you wanted to model the tent from flat, you cannot use linear modal methods. It is a time domain direct method where you 1st lift the tent ==> handle all sliders between the rods bending and cover sleeves and use NLGEOM=YES all over, and probably over tiny time increments.
A modal superposition method cannot do that, hence we reuse the original mesh with the right math for stiffness from preload.
I wouldn’t mix buckling into this debate as it can be linear or highly-non-linear.
1 Like
Also, the use of the word PERTURBATION confuses me here.
Traditionally in FEA, a perturbation step is 100% linear, then if you use nlgeom=yes, it can be non-linear if that’s what the setup wants to be.
Is that a CCX thing, to use perturbation keyword for a non-linear static step?
This is from the CCX user’s doc, there is no need to use nlgeom=yes; the latter is the Abaqus format, but not CCX, apparently.
in CalculiX frequency or modal analysis is nonlinear and used Newton-Raphson to solve in complex frequency analysis, but says similar with textbook for simple frequency analysis. However, it still shown questionable on my eigenbuckling test but i miiss something maybe.
p.s i have more intuition in buckling behavior than modal vibration, it can be verified in further also by large deformation analysis. Even each of them is different, still modeling process can be similar. Nonlinear buckling of metallic structure required geometric imperfection from deformed mesh and initial residual stress to be consider.
We are not doing modal superposition here. It is a simple frequency analisys.
Another aparently confirmation that Perturbation updates the geometry that will be used by the frequency solver.
It should be stiffness, not geometry, mixing things up.
You ARE doing linear modal methods as soon as you invoke the modal analysis (*Frequency).
Again, buckling can be a separate modelling, the static preload may be non-linear, but a (real, not complex form) modal run is always linear.
This is from the Abaqus docs:
NOTE the wording here: “stress & load effects”, not state; i.e. not absolute values are passed onto modal.
I see CCX is the same concept, only the stiffness effects get passed onto modal. See from user’s doc:
I think the keyword (switch) to account for preload seem different, but that is all.
Abaqus → nlgeom=yes in static step | CCX → perturbation keyword present in frequency step.
I have just uploaded a case where I have compared this question in the past.
And as already mentioned: CaluliX respects the pre-stressed case in the frequency step. Yes, the pre-deformed shape is not shown in the modal analysis (*1), but the modified geometry is respected. As in my case: the (kind of) pendulum is lengthened by the mass and so the natural frequency, shapes and order are changed. I only use linear materials, so the influence of the pre-stresses is negligible.
*1 As Sound_Spinning already mentioned: How do you want to compare the correct deformed displacement from a static load case with the not globally corrected scaled displacement from the modal analysis? The absolute value from modal analysis cannot be used, only the relative values at each node can be compared. Therefore, you cannot add or subtract them.
gravity_influence_on_MA.pmx (2.2 MB)
2 Likes
PrePoMax definitely plots frequency deformation/animation from an undeformed mesh. I see this could be a problem and I will look into the .frd file if there is any information if the frequency step was computed based on the pre-stressed model.
3 Likes