Software Use > FEM Coupling (HyperFEA)
ANSYS Eigenvalue Buckling + Modal Analysis - User defined analysis?
mraedel:
Hi Ryan,
with
--- Code: ---/SOLU
ANTYPE,0
PSTRES,ON
LSSOLVE,101 ! Static solution
FINISH
/SOLU
ANTYPE,1
BUCOPT,LANB,3,0,100,RANGE
LSSOLVE,101 ! Buckling solution
FINISH
/SOLU
EXPASS,ON
MXPAND,ALL,,,YES,,YES
LSSOLVE,101 ! Expansion Pass
FINISH
--- End code ---
I seem to get some reaction loads from the buckling solution as well. Since the static solution with prestress-effects is the input for ANSYS buckling solution this should be equivalent to the static load case reaction loads ?! Or are these element loads for the eigenform ?!
My problem is that this only seems to work for one load case. Unfortunately, I have multiple load cases in my model, lets say 4. I already do have a CDB-file containing the model, let's say model.cdb, and the load step files for the static analysis model.s101 ... model.s104.
So if I understand you correctly, for the static solution I can just copy my model.cdb e.g. to model_static.cdb. Additionally, I have to create 4 more copies for each buckling solution, e.g. model_buckling_LS101.cdb ...model_buckling_LS104.cdb, since ANSYS can only store one buckling solution in a rst-file. Afterwards, I perform all ANSYS solutions to obtain rst-files for each case. Is that correct?
Finally, in the Select Run Decks dialog in the project setup window I choose the static solution as the primary run deck with the equivalent rst-file. Afterwards, I add the additional buckling run decks (cdb+rst) for the buckling solution ?
Is that the way you propose?
Does HyperSizer notice that the models (nodes, elements, ...) are identical between the different cdb-files?
Btw, i know that NASTRAN allows static and buckling solutions in one bdf-file. Is it easier to integrate global buckling and modal solutions with NASTRAN in HyperSizer (just define different SUBCASEs in the bdf) ?
mraedel:
Hi,
I modified my model generation according to your proposal. I now have the following models and result files:
--- Code: ---! Static:
! LSSOLVE,101,104,1
model_sol_static.cdb
model_sol_static.rst
model_sol_static.s101
model_sol_static.s102
model_sol_static.s103
model_sol_static.s104
! Buckling:
! LSSOLVE,20X
model_sol_buckling_ls201.cdb
model_sol_buckling_ls201.rst
model_sol_buckling_ls201.s201
model_sol_buckling_ls202.cdb
model_sol_buckling_ls202.rst
model_sol_buckling_ls202.s202
model_sol_buckling_ls203.cdb
model_sol_buckling_ls203.rst
model_sol_buckling_ls203.s203
model_sol_buckling_ls204.cdb
model_sol_buckling_ls204.rst
model_sol_buckling_ls204.s204
! Modal:
! LSSOLVE,30X
model_sol_modal_ls301.cdb
model_sol_modal_ls301.rst
model_sol_modal_ls301.s301
model_sol_modal_ls302.cdb
model_sol_modal_ls302.rst
model_sol_modal_ls302.s302
model_sol_modal_ls303.cdb
model_sol_modal_ls303.rst
model_sol_modal_ls303.s303
model_sol_modal_ls304.cdb
model_sol_modal_ls304.rst
model_sol_modal_ls304.s304
--- End code ---
I imported all in the Select Run Decks dialog. The primary run deck is the static analysis. Buckling and modal solutions are selected as additional rund decks. So far, so good.
Again, I defined FEA Constraints in HyperFEA: Displacement constraints, eigenfrequency constraints and buckling constraints on the displayset of the overall model. I use effective laminates in my model. Since the bending stiffness of an effective laminate is computed as a smeared value from the membrane stiffness I defined all constraints to act on A11,A12,A66 and not the bending stiffness terms. Additionally I activated Stiffness Requirement, Membrane in the Failure Tab.
One improvement: The results of the modal analysis now shows up in the Iteration Report with the correct value.
Unfortunately, I can't get the buckling solution to show up. The buckling analyses with ANSYS are performed for all load steps. In the ANSYS log-files, the eigenvalues are given so I guess they are also present in the rst-file, but the result just won't show up.
Is there something else I have to toggle on in the Failure Tab or somewhere else?
UPDATE:
I tried everything with the buckling constraints, Aij, Dij, Stiffness Requirement Membrane, Stiffness Requirement Bending. If I only active the global buckling constraint, nothing happens: no eigenvalue, no Required Values for the stiffness terms in the Properties tab.
CDB-files for buckling and modal analysis are exactly identical, except the last lines, e.g. for load case 101=201=301:
Modal/eigenfrequency:
--- Code: ---/GO
FINISH
/SOLU
ANTYPE,2
MODOPT,LANB,3,0,200
LSSOLVE,301
FINISH
--- End code ---
Buckling:
--- Code: ---/GO
FINISH
/SOLU
ANTYPE,0
PSTRES,ON
LSSOLVE,201
FINISH
/SOLU
ANTYPE,1
BUCOPT,LANB,3,0,100,RANGE
LSSOLVE,201
FINISH
--- End code ---
The load step files *.s201 and *s.301 are completely identical. I know, I would not need the loads for the modal analysis, but they do no harm.
Ryan:
For the buckling solutions, you can verify if the RST file has the eigenvalue and mode shapes by plotting the mode shapes in the FEM Viewer. Data | FEA Mode Shapes. Also, HyperFEA will ignore buckling mode shapes with negative eigenvalues and with modal deflections whose max magnitude is less than 0.75 (typically the deflections are normalized to 1).
-Ryan
mraedel:
Hi Ryan,
thanks for the tip. I only calculate positive eigenvalues in ANSYS.
When I open the translation magnitude of Data | FEA Mode Shapes in FEMViewer I do see a buckling pattern. Btw, is this the one of the i-th iteration? The first eigenvalue is supposed to be 1.587 and the nodal deflections of the eigenform 4.02E-2mm.
So, I guess the buckling solution is in the rst-file. Why doesn't it show up in HyperFEA?
The help says:
--- Code: ---Modes with negative eigenvalues and modes with a max translation magnitude less than 1.0 are ignored.
Note the translation check is not performed for frequency constraints.
--- End code ---
Are my buckling cases ignored because the translation magnitude is too small? What is the meaning behind the limit of 1?
UPDATE:
I managed to get the buckling result into HyperFEA. For me an expansion of the ANSYS buckling solution was necessary. Why is this not necessary for the modal analysis?
Ryan:
Mode shapes are just "shapes", they do not have a real value for magnitude. Most solvers normalize the buckling nodal displacements such that the max magnitude of translation is 1.0. If the max magnitude of translation is not 1.0 it could be a sign of a spurious mode shape - some sort of solver issue - so HyperFEA will ignore it.
This check is only performed for buckling because the Nastran default for frequency mode shapes is to normalize by mass.
One thing I would do is verify that the buckling nodal deflections in the HyperSizer FEM Viewer are the same in the ANSYS APDL viewer. This would eliminate any chance that this is a unit conversion issue. I've verified the units behavior locally, but it is good to verify.
I'm not as familiar with ANSYS, but there may be some solver options to get the displacements normalized.
-Ryan
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version