Learning Forum

[RezaAlavi]

Can buckling appear in Static Structural analysis ? For example, if I have a column under vertical loading, if the critical load goes beyond the Euler critical buckling load, does the column buckle if we are ONLY in the Static Structural modulus of workbench, or it is necessary to use the Eigenvalue Buckling analysis as well ? I am asking this question, because I would like to know the deformation mechanism in more complex structures. For example, in an open cellular structure, (image attached) under vertical loading, can we differentiate which part of deformation in an strut was due to buckling and which part due to bending ?

   

[peteroznewman]

Yes, you can see buckling in Static Structural. Eigenvalue Buckling is a linear analysis. Static Structural is used to study nonlinear buckling and to study post-buckled behavior.

Eigenvalue Buckling takes a structure supporting a compression load and finds the load when the structure goes sideways (or snap-through for a dome). Static Structural can apply that same load by increments and the results can be animated to see the structure start compressing in-line and then go sideways. Static Structural can include nonlinear effects such as contact or plasticity that Eigenvalue Buckling cannot.

There is only deformation. It is not easy to separate, in a Static Structural model, the deformation due to "buckling" and the deformation due to bending. Why do you want to do that?

 

[RezaAlavi]

Thank you for your response. In some papers I have seen that the deformation mechanism of struts of a foam under compression is studied. However, those were conducting actual compression tests on the real foam samples and then analyzed the deformed struts after different levels of compression strains. I was curious if we could do such analysis via numerical modelling on idealized foam structure. That said, it is not a very crucial issue for me at the moment.

For the most part, I wanted to make sure whether Workbench takes into account buckling in Static Structural if the buckling takes place in single struts of a cell under compression . So, based on your answer, I understand that it does take into account the non-linear buckling (although the difference between linear and non-linear buckling is not still very clear to me). However, it is quite unclear to me that HOW the solver exactly does that (which method/algorithm it uses), so I hope I can find the theoretical information on Ansys Help (?). 

I ran a simple test on a slender column (1mx1mx100m) with Elastic material properties and fully constrained on one end. I applied a vertical compression load well beyond the theoretical critical Euler load for linear buckling. I did the analysis in Static Structural with large deflection on. However, I did not observe a buckling (significant horizontal movements normal to loading direction), and the deformation was only vertical aligned with the loading direction. How would you explain that ?    

[peteroznewman]

Any nonlinear analysis in Static Structural requires that Large Deflection be turned On. That is found under Analysis Settings.

A nonlinear buckling analysis in Static Structural has some tiny side load or some tiny amount of imperfection inserted into the geometry prior to beginning the analysis.

After you do these two things, you will see the structure buckle in Static Structural. When using an axial force to compress the column, you will find that when the load, which is incremented slowly, approaches the critical buckling load, the solver will fail to converge. That is because the Force-Deflection curve approaches a zero slope, so there is no static equilibrium at the next load increment.  If you switch from an axial force to an axial displacement to compress the curve, the solver will not fail to converge and when the reaction force is plotted vs the deflection, the force is seen to approach a maximum and then have a negative slope as the displacement continues to increase.

The linear Eigenvalue Buckling will compute a critical buckling load without having Large Deflection on or needing any side load or geometric imperfection added to the geometry.  The nonlinear Static Structural model will show the maximum force to be a lower value than the critical buckling load computed by the Eigenvalue Buckling solution. That is why the linear result is only useful as an initial result and the nonlinear Static Structural must be the next analysis to properly evaluate the sensitivity of the structure to imperfections.

[RezaAlavi]

I performed eigenvalue analysis, and the critical load was around 4.1E08N as I had obtained by hand calculation. Then, I applied non-linear Static Structural analysis by applying 8E08 N compressive load and a lateral 1N load on the edge. The dimension of the column was 1mx 1m x 10m this time. No deflection was observed and the the load was linearly increasing to the end. I do not understand why no buckling happened.

  

[peteroznewman]

I will take a look at your model. Please use File > Archive and save a .wbpz file. You can attach that after you reply. Say what version of ANSYS you are using in your reply.

[RezaAlavi]

Workbench 19.1

[peteroznewman]

I'm looking at your model in 19.2. if I run the Eigenvalue Buckling with no side load, I get a load factor of 122.8

Therefore, the critical buckling load would be 122.8*8e+8 = 9.824e+10 N. I didn't do a hand calculation for the bucking load.

Replacing the Force with a Remote Displacement, and unsuppressing the side load in a nonlinear Static Structural, after compressing to 1 m, the column has definitely buckled and the reaction force is 2.225e+10 N, significantly less than the critical buckling load found in the Eigenvalue solution.

If the Remote Displacement point is made eccentric by 0.25 m from the center of the column, it will buckle into the simpler Mode 1 shape at a much lower load.

Here is the Force-Time=Displacement curve that shows the buckling load was less than 4e+8 N.

[RezaAlavi]

Thank you. The discrepancy between your results and mine is due to the load factor and consequently the critical load which is much lower in my case.. The one you obtained is way larger than mine. I do not understand where the difference comes from. That said, the critical load I obtained is MUCH closer to the theoretical critical load obtained by Euler formula, i.e. Pcr= (Pi^2) EI/ (2L)^2 for a one-end totally constrained column. Can I have your file so I look at it in detail and understand where we did differently? 

[peteroznewman]

You are welcome to the file, but I used ANSYS 19.2 so unless you have that or later, you can't open the file.

This column is very thick so is far from the slender column that is assumed by the Euler formula.

As the cross-section of the column becomes more slender, the ANSYS result will begin to approach the Euler formula.

[peteroznewman]

I did a slender column, the cross-section is 0.2 x 0.2 m and the length is 10 m with Steel where E = 200 GPa.

I used this website to compute the Euler solution. The critical buckling load is 596.8 kN.

The ANSYS Eigenvalue Buckling solution for that load was a Load Multiplier of 1.1 so the critical buckling load is 656.5. kN, which is about 10% over the Euler solution.

The model was copied to a Nonlinear Static Structural model where a Remote Displacement on the 200 x 200 mm top face was offset by 1 mm from the center to provide a small eccentricity to seed the buckling along the x axis.  Here is the force-time plot where at t=1, the vertical displacement was 2 mm. You can see that the force is 653 kN, which is very close to the Eigenvalue result of 656.5 kN.

An ANSYS 19.1 archive is attached since I was able to switch to another computer that has your version installed.

[RezaAlavi]

 Thanks a lot. Thanks to your examples, I have a far better understanding of buckling modeling in Ansys. Similar to your last examples, I modeled a slender column (1mx 1mx 80m). First I derived the critical load through Static Structural in conjunction with Eigenvalue, and it was  6.4307e+006 N. Then, I conducted Nonlinear Static analysis with remote force. When I applied the remote force (compressive 6.4E06 N)  on an eccentric remote point (only 1mm offset from the centre of the top face), I observed the following total-deformation_time diagram. However, the force was linearly and monotonically increasing. The onset of instability corresponds to the reaction force of 6.08e+006 N. 

  

[RezaAlavi]

Why should we introduce eccentricity or other types of imperfection in order to observe the buckling in Nonlinear Static ? And why did you prefer to use remote displacement as opposed to regular displacement on the surface ?

 

 

[peteroznewman]

A remote displacement makes it very easy to introduce an eccentricity into the load.

A remote displacement leaves all other DOF free.  A displacement on the top face requires that the face normal remain parallel to the Y axis, so it can't rotate the way a remote displacement can.  A free end implies that the top can rotate a little as it goes sideways.

Engineers design for the worst case buckling load, which means the lowest buckling load. That occurs at the worst case eccentricity.  If you design for the worst case, then you build the structure with less eccentricity than the specified worst case, the structure has a good margin to the actual buckling load. 

You don't want to do the opposite, use no eccentricity in the analysis and claim the column can support some large load, then find out the structure failed at a lower than predicted load because the structure was built with some eccentricity. Nothing is built perfectly.

If your original question has been answered, please mark the post that best answered the question with Is Solution (while you are logged in). This will mark the discussion as Solved.  You can open a New Discussion if you have new questions, or ask a followup question here.

[Yuvarajan C]

Does the deformation remain the same in eigenvalue buckling for the increasing load ? If no what to do?