{"id":25657,"date":"2011-03-24T09:38:00","date_gmt":"2011-03-24T09:38:00","guid":{"rendered":"https:\/\/www.padtinc.com\/2011\/03\/24\/ansys-13-0-enhanced-modal-analyses-with-linear-perturbation\/"},"modified":"2022-03-31T14:14:53","modified_gmt":"2022-03-31T21:14:53","slug":"ansys-13-0-enhanced-modal-analyses-with-linear-perturbation","status":"publish","type":"post","link":"https:\/\/www.padtinc.com\/2011\/03\/24\/ansys-13-0-enhanced-modal-analyses-with-linear-perturbation\/","title":{"rendered":"ANSYS 13.0 Enhanced Modal Analyses with Linear Perturbation"},"content":{"rendered":"

\u201cRest, rest, perturbed spirit!\u201d\u00a0 – William Shakespeare<\/p>\n

If you have ever performed a large deflection prestressed modal analysis in ANSYS Mechanical APDL prior to version 13.0, your spirit might have been perturbed as well.\u00a0 The procedure was not very user friendly, to sum it up.\u00a0 For example, unless you were careful, the modal results would over-write the static preload results.\u00a0 Thankfully, at 13.0 we have a smoother and more capable tool for handling large deflection prestressed modal analyses.\u00a0 This new procedure is called Linear Perturbation.<\/p>\n

We\u2019ll focus on modal analyses in this article, but be aware that linear perturbation also applies to linear buckling analyses at 13.0, but only following a linear preload solution, and only in Workbench.\u00a0 The capability for modal analyses is supported in both Workbench and Mechanical APDL.\u00a0 Also, the preload, or \u2018base\u2019 analysis has to have multiframe restart capability turned on.\u00a0 This will happen by default for a nonlinear analysis but needs to be manually activated in MAPDL for a linear analysis by issuing the command RESCONTROL,LINEAR.<\/p>\n

In fairly simple terms, the prestress effects are included in a modal analysis via the change in the stiffness matrix that occurs during the prestress (typically nonlinear static) analysis.\u00a0 This is the method that has been used in ANSYS for years.\u00a0 What\u2019s new at 13.0 is that the program keeps track of different components of the augmented tangent stiffness matrix.\u00a0 The five possible contributing components are material property effects, stress stiffening effects, load stiffening effects, contact element effects, and spin softening effects.<\/p>\n

While the material effects must remain linear, the contact stiffness can be altered, if desired, in the subsequent modal analysis.\u00a0 More on that later.<\/p>\n

The typical Mechanical APDL procedure to perform a nonlinear static structural prestress run followed by a modal analysis which utilizes those prestress effects is as follows:<\/p>\n

! With static model prepared<\/p>\n

\n

\/solu\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! enter solution module
\nantype,0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! specify static analysis type
\nnlgeom,1\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! turn on large deflection effects (nonlinear)
\npstres,on\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! turn on prestress effects for subsequent modal
\nnsub,10,10,10\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! specify substep range
\nsave\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! save the database
\nsolve\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! solve the nonlinear static prestress case
\nfinish\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! leave the solution module
\n\/solu\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! re-enter solution so we can do a new analysis
\nantype,,restart,1,10,perturb\u00a0\u00a0\u00a0\u00a0 ! specify restart option for linear perturbation
\n! from last substep in this case
\nperturb,modal\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! specify modal as next analysis
\nsolve,elform\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! calculate element formulation with solve command
\nmodopt,lanb,12\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! specify modal options for solution
\nmxpand,12\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! specify number of modes for results calc
\nsolve\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! solve the prestress modal analysis
\n\/post1\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! enter general postprocessor
\nINRES,ALL\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! make sure we read in all results from file
\nFILE,’nonlinear_static’,’rstp’\u00a0\u00a0 ! specify special results file for modal results
\nset,first\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! read in results for first mode
\nplns,u,sum\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! plot mode shape
\nset,next\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! read in results for next mode
\n\/repl\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 ! plot mode shape, etc.<\/p>\n<\/blockquote>\n

 <\/p>\n

Note that the linear perturbation (modal) analysis has its own results file, the .rstp file.\u00a0 Because of this, the preload results are still available in their own .rst file as it does not get overwritten by the modal step.<\/p>\n

Here is a table of frequency results for a simple test case.\u00a0 Three modal analyses were run:<\/p>\n

1.\u00a0 No prestress at all.<\/p>\n

2.\u00a0 With a linear static prestress state.<\/p>\n

3.\u00a0 With a nonlinear static prestress state.<\/p>\n

\"image\"<\/a><\/p>\n

Here is the model used for these runs in its initial configuration.\u00a0 The block at the base was fixed in all DOF\u2019s and the preload applied was a pressure load on one side of the vane.<\/p>\n

\"undeformed\"<\/a><\/p>\n

Here is the model with the deformed mesh due to the nonlinear prestress:<\/p>\n

\"nonlin_prestress_deformed\"<\/a><\/p>\n

Here is a mode shape plot for mode 12:<\/p>\n

\"nonlin_prestress_mode12\"<\/a><\/p>\n

The above example is all well and good but could have been done in prior versions of ANSYS using the old partial solve method.\u00a0 What\u2019s nice about the newer linear perturbation method is that it\u2019s easy to get the mode shape plots relative to the deformed mesh from the prior prestress run, and you don\u2019t need to worry about over-writing the prestress results with the modal results, since the corresponding results files are different.<\/p>\n

Further, we can now perform modal analyses using different restart points in the static prestress run, assuming multiple restart points are available.<\/p>\n

Finally, we can actually change some contact options between the static prestress solution and the modal solution.\u00a0 For example, if the prestress analysis was run using frictional contact, the subsequent modal analysis can be run utilizing the prestressed state of the structure but with one of three contact states for the modal analysis: true status (that of the prior static analysis), force (to be) sticking, or\u00a0 force (to be) bonded. The sticking option applies only to contact elements with a nonzero coefficient of friction. The bonded option will force contact pairs that are in contact in the static analysis to be bonded in the modal analysis.<\/p>\n

The Mechanical APDL command sequence for this procedure would be something like this:<\/p>\n

 <\/p>\n

! first perform nonlinear static prestress run, then<\/span><\/span><\/p>\n

\/solu<\/span><\/span><\/p>\n

antype,,restart,,,perturbation<\/span><\/span><\/p>\n

perturb,modal,,BONDED,PARDELE\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 <\/span>! pre-stress modal analysis, switch contact to bonded, delete <\/span><\/span><\/p>\n

\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 <\/span>! loads in case future MSUP<\/span><\/span><\/span><\/p>\n

solve\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 <\/span>\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 <\/span>! Generate matrices needed for perturbation analysis<\/span><\/span><\/p>\n

! Next perform modal analysis<\/span><\/span><\/p>\n

modopt,lanb,6<\/span><\/span><\/p>\n

mxpand\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 <\/span>! default expand in case of complex solution<\/span><\/span><\/p>\n

solve<\/span><\/span><\/p>\n

! modal results are now available for postprocessing<\/span><\/span><\/p>\n

\n

In Workbench Mechanical, the appropriate command sequence is sent to the solver when we link a modal analysis to a prior prestress analysis.\u00a0 If the model involves contact, then in the modal analysis we\u2019ll have choices for how the contact should be treated in the Pre-Stress branch under the Modal branch in the Outline Tree.\u00a0 For frictional contact in the static prestress analysis, the choices in the Details view for the Pre-Stress branch in the modal analysis will be Use True Stress, Force Sticking, or Force Bonded as described above.<\/span><\/p>\n

\n

Here are some example plots for this scenario:<\/span><\/p>\n

\n

Two 3D plates subject to in plane bending, fixed at right ends, frictional contact between them.<\/span><\/p>\n

\"image\"<\/a><\/p>\n

\n

Resulting contact status for static run (sliding is occurring)<\/p>\n

\"image\"<\/a><\/p>\n

Resulting static deformation:<\/p>\n

\"def_c\"<\/a><\/p>\n

 <\/p>\n

Mode 6 result, \u201ctrue\u201d contact behavior:<\/p>\n

\"mode6_nonlin_true_c.\"<\/a><\/p>\n

 <\/p>\n

Mode 6 result, \u201cforce bonded\u201d contact behavior:<\/p>\n

\"mode6_nonlin_force_bonded_c\"<\/a><\/p>\n

Those last two images show a dramatic difference in modal results simply by changing the contact status behavior in the modal analysis.\u00a0 In the first of those images, the contact status is set to \u2018true\u2019, meaning essentially the same as in the prestress analysis, subject to the linear nature of the modal analysis.\u00a0 In this example, the frictional behavior in the static prestress run becomes no separation in the modal analysis, so the two plates can have mode shapes in which the plates slide relative to each other.\u00a0 In the last plot, the contact status has been changed to \u2018force bonded\u2019 for the modal solution.\u00a0 As the plot shows, mode shapes can only exist in which the two plates are bonded together.\u00a0 Both modal analyses have the same prestress condition however.<\/p>\n

Here is a frequency table comparing the first six modes of the two modal analyses.\u00a0 Note that with the contact forced to be bonded we get a stiffening response as we might expect.<\/p>\n

\"WB_freq_compare\"<\/a><\/p>\n

So, although on the surface it might initially appear to be a black art, linear perturbation is a nice enhancement in ANSYS 13.0 that gives us a more robust and capable method for performing modal analyses with prestress effects included.\u00a0 The prestress run is typically a linear or nonlinear static analysis, but it will also work with a full transient analysis to define the prestress state.\u00a0 The ANSYS 13.0 Help has more information (see section 9.2 of the Mechanical APDL Structural Analysis Guide and section 17.8 of the Theory Reference).\u00a0 We also recommend you try out the procedure on your own models.<\/p>\n","protected":false},"excerpt":{"rendered":"

\u201cRest, rest, perturbed spirit!\u201d\u00a0 – William Shakespeare If you have ever performed a large deflection prestressed modal analysis in ANSYS […]<\/p>\n","protected":false},"author":4,"featured_media":0,"comment_status":"open","ping_status":"open","sticky":false,"template":"","format":"standard","meta":{"footnotes":""},"categories":[2323],"tags":[],"post-podcast":[],"_links":{"self":[{"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/posts\/25657"}],"collection":[{"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/posts"}],"about":[{"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/types\/post"}],"author":[{"embeddable":true,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/users\/4"}],"replies":[{"embeddable":true,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/comments?post=25657"}],"version-history":[{"count":0,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/posts\/25657\/revisions"}],"wp:attachment":[{"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/media?parent=25657"}],"wp:term":[{"taxonomy":"category","embeddable":true,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/categories?post=25657"},{"taxonomy":"post_tag","embeddable":true,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/tags?post=25657"},{"taxonomy":"post-podcast","embeddable":true,"href":"https:\/\/www.padtinc.com\/wp-json\/wp\/v2\/post-podcast?post=25657"}],"curies":[{"name":"wp","href":"https:\/\/api.w.org\/{rel}","templated":true}]}}