turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Help with Inelastic Column Buckling with Material ...

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-16-2016 03:37 AM

Hi,

In my efforts to understand inelastic buckling, I decided to start with simple verifyable cases for which closed form solutions exist in the literature.

The easiest case I could think of was a 1D column with Simply Supported (Hinged) end conditions subjected to an axial compressive load.

The Cross Section details of the column is as follows:

The length of the column is 10 inches.

Material of the column is 2024-T3 Extrusion.

Since the end conditions are hinged, the effective length (Le) is also 10".

Ratio of Le/Rho = 10/0.2 = 50

I calculated the critical buckling stress (initially) using the expression Fcr = (pi()^2*E)/(Le/Rho)^2.

I got a value of 42240 ksi, which is greater than yield stress of the material (Fcy = 40 ksi). The corresponding critical load = 42240 x 0.502 = 21204 lbs

The plasticity correction has to be factored in. Refering Bruhn Vol.2 Chapter C2, Fig C2.17, I was able to figure the actual critical buckling stress as close to 30.5 ksi.

The critical buckling load = 30500 x 0.502 = 15311 lbs.

I set out to perform the above analysis in Femap using SOL 106. I applied a small moment around Mz axis of value 25 lbs-in to provide the initial imperfection that is needed to induce buckling.

The Nonlinear settings is as follows:

For the material properties, a hardening model was chosen (unsure if chosen model can be applied to buckling).

The analysis runs fine but I get buckling load as around 21250 lbs and wierd stress values.

Whats up with the insane 348,269 psi value? Or should stress output vectors not be consulted when nonlinear buckling analysis is conducted?

More importantly, Femap is not providing me the revised critical buckling load of 15300 lbs per my hand calculation.

I am sure FEA packages are capable of capturing inelastic buckling phenomenon, but it seems like I am missing something in the above procedure.

Would appreciate more experienced members suggesting pointers on accomplishing my end goal.

Thanks in advance.

10 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-16-2016 08:58 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-16-2016 10:23 AM

I would suggest looking at your F06 file to understand more about how this nonlinear analysis proceeded in the solver. While I don't have your actual model, I tried to follow your inputs as posted. The first thing I notice in the F06 is the following message:

*** USER WARNING MESSAGE 23201 (TA1NLE)

CBEAM ELEMENT 1 DOES NOT SUPPORT ANY NONLINEAR MATERIAL OTHER THAN ELASTIC-PERFECTLY PLASTIC

LINEAR MATERIAL WILL BE USED INSTEAD

So, I believe in reality Nastran ended up using a linear material.

As far as the stress values, are you plotting converged results? I notice the "time" is < 1.0, if this is the last result, then the run did not converge to the end of the specified loading. If the step you plotted is not a converged result, then the numbers really have no meaning.

We normally consider a model "buckled" in a nonlinear run when the following message appears in the F06:

*** USER WARNING MESSAGE 4698 (DCMPD)

STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .

THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN

1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.

Find the first load increment or "time" where this occurs to understand where instability starts.

For my run, using your inputs as posted, I see this message occur when the load reaches 2250lbs. My solution does converge at this load level, however I see very high stress values at this level, since Nastran actually used a linear material model.

When I switch to a elastic-perfectly plastic material model by changing to "plastic" as shown below, then look at converged stress results, I believe your answers will be more like you expect.

Hope this helps

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-17-2016 05:09 AM - edited 06-17-2016 05:18 AM

Fembrackin,

Thanks for the valuable insights on buckling. Perhaps, I should start paying more attention to messages in F06.

"*** USER WARNING MESSAGE 4698 (DCMPD)

STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .

THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN

1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL."

If I don't mind asking, where can I find the above in the official literature?

I will incorporate the changes i.e. make the material perfectly plastic and see if I am able to obtain much more accurate results.

Spatrashi,

The Cross Section of the column I have is stable i.e. not open or unstable. Further, the end fixity conditions of the column are such that it does not prevent global buckling. Hence there will be no local buckling or crippling for this type of cross section column.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-17-2016 06:10 AM

Fembrackin,

I tried incorporating changes you have suggested and still unable to obtain results which match hand calculated ones.

Is it possible for you to post a copy of your dat file (or femap model file) so that I can examine closer your results and procedure?

Thanks

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-17-2016 10:20 AM

I have attached the 2 dat files. One is for the bilinear material model which generates the warning messages. The other is for pefectly plastic material model.

I think part of your issue is which set of results you choose to plot. Make sure you requested intermediate results so you see results at each load increment.

For your original model, do not look at results for load step 1.0( my model did converge all the way out to 1.0), back up to the step where the instability first occurs, that is the buckling load, you can get solutions after that, but now you are in"post-buckling" behavior and maybe even unconverged results, must inspect the f06 to determine this.

When you run the perfectly plastic case, the column actually collapses shortly after the critical buckling load is reached, the solution stops after .772 and gets a fatal error after that.

Notice I also changed the iteration settings to method of "ITER" with an update of 1, this means the stiffness is updated after every iteration.

Regards,

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-18-2016 02:59 PM - edited 06-18-2016 03:09 PM

Fembrackin,

Thanks for posting the files. I really appreciate it.

I had a chance to go through it and I have a few questions about your approach.

Like you have mentioned, in your plastic analysis, how do you determine the critical buckling load based on output case? The below screenshot is from post processing window of your perfectly plastic run.

Also, I ran my model with an axial compressive load of 100,000 lbs with Stiffness updates method set to ITER & iterations before update set to 1. At case 6, load factor of 0.1968, the column assumed bent shape and at case 7, load factor of 0.2, the column collapsed. I am assuming that critical buckling load is 0.1968 x 100,000 = 19680 lbs, which is still higher than the load from hand calculation (15300 lbs).

I do really appreciate your efforts in trying to help/resolve this issue for me. I wish Femap folks do a webinar or a video illustrating the steps of performing an inelastic column buckling like they have done an excellent job with other topics.

Thanks again!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-20-2016 10:22 AM

With "ordinary" sol 106 nonlinear static analysis, the load ramping is not used. Just apply the total desired load, Nastran internally scales the load according to the number of increments that you request. So, 10 increments means we apply 10%,20%,30%, etc.

For Advanced nonlinear solutions, load ramping is required, so you must creat the "time history" function and reference it on load definition. In advanced nonlinear the you input number of increments and also the "time increment" to get the total time of the analysis.

To determine the value of the critical load, we can look in several places. Being an "old user", I always start by looking at the f06 file. By looking at the iteration summary printout, we look for the first load increment where we get the negative matrix diagonal factor. From my bilnear material run I see the following:

0 N O N - L I N E A R I T E R A T I O N M O D U L E O U T P U T

STIFFNESS UPDATE TIME 0.01 SECONDS SUBCASE 1

**ITERATION TIME 0.00 SECONDS LOAD FACTOR 0.8000000**

- - - CONVERGENCE FACTORS - - - - - - LINE SEARCH DATA - - -

0ITERATION EUI EPI EWI LAMBDA DLMAG FACTOR E-FIRST E-FINAL NQNV NLS ENIC NDV MDV

1 1.5919E+01 1.0088E-01 1.4249E-02 1.0000E-01 4.9044E+00 1.0000E+00 5.7070E-02 5.7070E-02 0 0 0 1

*** USER INFORMATION MESSAGE 4550 (NCONVG)

*** NEW STIFFNESS MATRIX IS REQUIRED ***

User information:

This is issued based on the stiffness matrix update strategy specified

on the NLPARM or TSTEPNL entry, or when the adaptive gap element stiffens

or its penalty value is adjusted after convergence.

*** SYSTEM INFORMATION MESSAGE 6916 (DFMSYN)

DECOMP ORDERING METHOD CHOSEN: DEFAULT, ORDERING METHOD USED: MMD

***** USER WARNING MESSAGE 4698 (DCMPD)**** STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .**** THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN**** 1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.**

So, I know that at 70% load there was no message, at 80% load I am unstable. I do not know exactly the value, only that it is between 70% and 80 % of my applied load of 25000 lbs. All I really know is that the critical load is between 17500 and 20000. If I had used a larger applied load, then my "uncertanty" would be higher. If I need to know more precisely the critical load, then I can increase the number of increments to 20, now my load steps are 5%.

You can also get a better understanding by looking at a chart of tip displacement vs load step value. see the pictures below:

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-21-2016 03:16 AM

Thank you Sir.

Those are indeed some valuable insights on buckling interpretation.

I am exhausted trying to get a FE buckling result which matches my short column hand calculated ones.

Since this is for my learning, I will postpone it till I need it.

Appreciate your help so far.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-21-2016 10:12 AM

Sorry you feel exhausted by this topic.

Here is a suggestion to improve your results. Instead of using the end moment, try perturbing your geometry by the linear buckling mode shape. This is a somewhat standard approach and in your case it gets better agreement with the charts from Bruhn.

This process is made very easy in Femap. Under "Custom Tools" go to "Postprocessing" and then to "Nodes Move by Deformation with Options"

I used this tool and updated the X and Z coordinates using a scale factor of .01 on the linear buckling mode shape. Now using the elastic-perfectly plastic material model and a compressive load of 25000 with 10 load increments, the critical load is approximatly .625*25000=15625

The plot below shows good agreement (31081psi vs 30500psi) with the critical stress values obtained from Bruhn also.

Regards,

Joe

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc