ANSYS Eigenvalue Buckling + Modal Analysis - User defined analysis?

[mraedel]

Hi,

I would like to incorporate a global linear buckling and modal analysis in my sizing using ANSYS. HyperFEA allows the definition of a buckling constraint in the Global FEA Constraints. Unfortunately, it seems not to be implemented yet for use with ANSYS.

I wonder, is it possible to start a linear buckling analysis from HyperSizer using an APDL-script and read the result in HyperSizer using the "User defined analysis"?

[Ryan]

Hi,

We have implemented a new global buckling constraint feature in V7.1 (currently in beta). Attached is a description of this new feature.

1) The location of the buckling mode is automatically detected within a display set based on the grid displacements.
2) Required stiffness factors are applied per mode, per component based the relative grid displacement.
3) All modes shapes can be displayed in the FEM viewer.
4) Frequency constraints have been added as well. The algorithm is identical to the one used for global buckling.

We may be able to distribute a beta version of V7.1 to you. I will contact you offline for more details.

Thanks,
Ryan

[mraedel]

Sounds promising.

I am looking forward to hear from you.

[mraedel]

Hi, I now use HyperSizer 7.1.43 which should support global buckling and modal analysis. So, I used HyperFEA, created a FEA Constraints for buckling and eigenfrequency on a displayset containing the whole model. I additionally use displacement constraints.

When I start HyperFEA, everything works. The displacement constraints act as expected. But unfortunately, in the Iteration Report Constraints tab I see, that the actual eigenvalue for buckling and the actual eigenfrequency of the iteration are zero.

Does this mean no buckling and modal analysis was performed? I have no real idea how to tell HyperSizer to perform a global buckling anaylsis in ANSYS.

I re-read the attached word-file from your previous answer and read the sentence "The project must include the run deck with the buckling solution. Modal grid displacements must be exported to the relevant FEA results file."

Does this mean I have to provide buckling results in the initial ANSYS rst-file at import? How do I tell ANSYS to write these buckling results in the same rst-file as the static solution?

The import of load sets is described here. When I try to use

Code: [Select]

/SOLU
LSSOLVE,101      ! Static solution with PSTRES,ON
LSSOLVE,201      ! Buckling
FINISH

I get an error in ANSYS:

Code: [Select]

The analysis type must not be changed after the first load step.  For a
new analysis, enter the FINISH command now and reenter using the
/SOLUTION command.

But if I use

Code: [Select]

/SOLU
LSSOLVE,101      ! Static solution with PSTRES,ON
FINISH
/SOLU
LSSOLVE,201      ! Buckling
FINISH

the calculation is done, but the rst-file of the static solution is overriden by the buckling solution and I can not import the reaction loads for the static load case in HyperSizer.

Is there a simple exemplary CDB-File with load step data or an APDL file to show the process?

[Ryan]

We've seen this too. To the best of our knowledge, you can't have an ANSYS result file (RST) with both static (perturbation) and buckling results. This appears to be a limitation of the RST format in ANSYS.

The workaround would be to make separate run decks  - one with static, and another with static + buckling. You can use include statements to share model, loads, and boundary condition data between the two run decks.

-Ryan

[mraedel]

Hi Ryan,

with

Code: [Select]

/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

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: [Select]

! 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

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: [Select]

/GO
FINISH
/SOLU
ANTYPE,2
MODOPT,LANB,3,0,200
LSSOLVE,301
FINISH

Buckling:

Code: [Select]

/GO
FINISH
/SOLU
ANTYPE,0
PSTRES,ON
LSSOLVE,201
FINISH
/SOLU
ANTYPE,1
BUCOPT,LANB,3,0,100,RANGE
LSSOLVE,201
FINISH

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: [Select]

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.

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

[mraedel]

Sure, the buckling shapes are just the result of the deformation for the eigenvalue inserted in the eigenvalue problem/shape functions. In general in ANSYS this does not seem to be normalized to the mass.

I did verify the deformations and they look appropriate.

The expansion pass in ANSYS seems to do the necessary calculation of the normalized displacements.

[mraedel]

I was happy too soon.

ANSYS performs the eigenvalue buckling analysis for all 4 load cases. I can display the requested modes for all load cases in the FEMViewer with the corresponding eigenvalue in the title.

Lets say I have the following results:

Code: [Select]

Load case 1: critical eigenvalue: 2.5
Load case 2: critical eigenvalue: 1.9
Load case 3: critical eigenvalue: 1.8
Load case 4: critical eigenvalue: 1.7

But, now my problem: in the Iteration Report of the FEMViewer the MAXIMUM eigenvalue is shown as lambda_actual, here 2.5. Is that just a wrong display and internally  minimum eigenvalue is used for the calculation of required stiffnesses? Or is just the value of the first load case displayed? Or is the inverse of the eigenvalue actually needed here?

On the other hand: Everything works fine for the eigenfrequencies. The minimum of all 4 load cases is found. But that might just be a coincidence, because the smallest eigenfrequency is present in load case 1.

Code: [Select]

Load case 1: first eigenfrequency: 60.0
Load case 2: first eigenfrequency: 70.5
Load case 3: first eigenfrequency: 70.2
Load case 4: first eigenfrequency: 71.1

I tried the following: I switched the model, load case and result files of load case 1 and 3 (renamed the files) for the stability and modal analysis. Thus, now the maximum buckling eigenvalue and the minimum frequency are in load case 3. The minimum buckling eigenvalue is still in load case 4.

The result is the following:

• The wrong minimum modal eigenfrequency 70.2 from the current load case 1 is shown
• The wrong critical buckling eigenvalue 1.8 from the current load case 1 is shown

Thus, my conclusion: The buckling and modal eigenvalue and eigenfrequencies are always obtained from the first load case, no matter which one is critical.

Is this a bug or did I do something wrong?

[Ryan]

Since eigenvalue 2.5 was reported in both scenarios, it sounds like the modes from load cases 2-4 are being filtered out due to the normalized deflections. You could confirm this by running with only a single buckling run deck.

-Ryan

[mraedel]

I do not think so. The maximun normalized deflections for all load cases are >1 in the FEM Viewer.

Also, I guess it was misunderstanding what I wrote. When I switched load cases 1 and 3, the printed buckling eigenvalue was 1.8, so still not the minimum, but the eigenvalue of the current (after the switch) load case 1. If your assumption would be the case, the printed eigenvalue should still be 2.5 . I updated my previous answer.

[Ryan]

I believe we found the issue. There is an issue with the reporting logic - for multiple buckling run decks. If all eigenvalues are greater than the limit, the first eigenvalue is reported as the minimum. If any eigenvalue is below the limit, the correct minimum eigenvalue is reported. This issue does not affect the optimization logic.

-Ryan