Greetings,
I am having troubles figuring it out, if frequency step on deformed structure due to previous static step is even possible? So far, the only thing that I have been able to do is to include the prestressed state into the frequency step, but i was unable also transfer the deformation?
Did you use the Perturbation option on the Frequency step, which applies preloads from the previous steps?
And make sure Nlgeom is enabled in the preload step. Theoretically, it may not be necessary in CalculiX but Abaqus needs it and it might be better to keep it.
Thanks for the replies. I did both, and I see that there are changes in natural frequency, however I think this is only due to stress stiffening effect. When i take a look at the results, I can see mode shapes oscillating around undeformed shape, not the one that has been obtained in the static analysis step.
My problem involves a structure similar to a thin beam, that is first deformed into an arc, and I want to calculate natural frequencies of that deformed arc.
Iâve also checked the Calculix manual and some forums in the mean time, and it seems that performing eigenvalue analysis on deformed shape is not possible.
Is there a reason why you want to do this with 2 steps? Why are you not saving the deformed mesh from step 1 and make a new simulation with this mesh that will handle your second step?
I agree with NorbertH especially if your making proces significa,tly change the shape of your beam.
I did not know that you can export deformed mesh. Iâve tried that and it works great, thank you!
On the side note, now I am not including stress stiffening effects, but for now the solution you guys proposed will work great.
In Abaqus, you can do it in the same analysis:
The same model in CalculiX (and the same scale factor):
Although the frequency values are in agreement.
So if I understand you correctly, youâre thinking that Calculix takes deformed state also into account, but the deformed state is not plotted in PrePoMax, just mode modeshapeâs relative deformations?
More tests would be needed (like the aforementioned approach with exported deformed mesh) but itâs possible that CalculiX displays the frequency step results with respect to a different base state than Abaqus.
I would agree with you. From my understanding of the ccx code, the base state is the undeformed state- but I could be wrong. It would be good to double check with both methods to confirm that is the case.
I also use the frequency step after a static step. In my case itâs only gravity that deflects the part. But I can say: yes, in calculix there is an influence of the pre-static load case on the natural frequency.
In the animations above, I think, you are comparing on both the lateral mode, which is not the one with the preload in Z. For that one is the same mass & stiffness, hence the same freq.
You should compare the 1st ânoddingâ mode in Z, which is the one with the preload direction to show higher freq.
Manual says âBy using the parameter PERTURBATION on the *STEP keyword card the user speciďŹes that the deformation and stress from the previous static step should be taken
into account in the subsequent frequency calculation.â
Deformations should be taken into consideration in the analisys too but there is something weird Âżisnât it?
In case the frequency analisys has some rigid body motion, the base geometry shown should be the deformed mesh result of the First step not the initial mesh.
I also think there is a problem . Maybe the import from the frd geometry should be the deformed mesh not the initial.
-I have an idea how to test. Does Prepomax respect the node numbers when the mesh is transfered to generte a new deformed mesh?.
?Âż?Âż. Why is the undeformed view of the first mode Step 2 (Frequency) different from the last true scale shape of the first step (NLGEOM) ?
Model BC and loads is inspired on benchmark Popular Benchmark Problems for Geometric
Nonlinear Analysis of Shells Figure 5a. Hemispherical shell. It is well deformed and model becomes much more rigid than the hemispherical undeformed shape.
K.Y.Sze1*, X.H.Liu1#, S.H.Lo2
The University of Hong Kong, Pokfulam Road, Hong Kong SAR, P.R.CHINA
I just add a new Frequency Step with peturbation parameter on and respecting same BC.
The disps do not get passed over static â modal, but the stiffness matrix contribution.
This is coz we cannot mix freq domain stuff with (real only) static disps stuff. Itâll get really confused in a forced response.
Is the same in all other FEA solvers Iâve used, including Abaqus. The stiffness is correct, and then you have to perform a (modal based) forced response (freq or time domain) to really compare the stiffness contribution from a static prestress into linear dynamics; with static vs w/out.
Also note that a modal analysis does not have loads is normalised (either disp or mass normalised); so static absolute disps do not make sense to be mixed, the [K] matrix contribution is correct coz it is in reality normalised.
But I donât suggest mixing displacements. I thought Perturbation takes the whole new geometry. New node coordinates to work with Âżisnât it?. Maybe Iâm reading the manual wrong. 
It doesnât need to, the [K] matrix is enough and mass doesnât change, remember modal et all is linear disps theory. The shape wouldnât make sense onto the modal, what values would you use?
If you are thinking of seriously non-lenear preload with large rigid body like rotations/distortions, that is a separate matter, youâll have to use the direct method in dynamics and not modal approaches.
Having said all that, there is a dirty trick to do (nearly) what you want into the forced response results. You drive the modal superposition run at very close to zero Hz with your static loads as real component input only. That time/freq step will give you the shape you are after, then the âactualâ forced response in the freq or time domain can have dynamic loads added to the static ones; but it is dirty, but it may work.
If you are interested in final stresses what we used to do is to solve the real dynamic job and with a script add the static preload disps/stress values on top, like a DC offset on a sine wave.
When previous step did not deformed at all, can it be stressed? perturbation is related to stress I guessed, not geometry after deformation. Try to change the case to eigenbuckling may give correlation. Insignificant deformation but reversed sign also.
