Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Simulating Euler buckling of simple column
Hi, I'm am rather new to Mecway and am looking for some help interpreting the results of my buckling analyses. My end goal is to determine when buckling occurs at an opening in a tubular structure. To get familiar with Mecway I first started by verifying stresses versus hand calcs, which all worked out fine. Then I moved on to check buckling of a simple round tubular column so that I could try to understand the results I was seeing. I'm not sure I understand what I'm seeing with the buckling results. The questions below and the attached file are for my buckling test column.
Note: The attached file has a vertical load input of 0.97x the Euler buckling load (Fcr). I listed all numerical values below as percentages of Fcr to avoid anyone having to do any unit conversions to understand what I'm saying.
I am using hex8 elements so that I can try both Buckling3D and Nonlinear Static 3D analyses. I have rigid plates on each end of the tube with pinned constraints and a concentrated vertical load applied to the center of the top plate. To initiate buckling I have placed a small horizontal near the midpoint of the column. If you want to skip the seemingly inconclusive tests, go to the last "**" below.
I started first with a --Buckling3D-- analysis:
**Using the I'm not sure what shift point to use. The warning that appears when you have the shift point at "0" says to set the shift point to a value between zero and the lowest buckling factor. But whatever shift point I input seems to be very close to the buckling factor listed in the results and all of my buckling factors are within 1% of each other. Do I need to start at a high shift point and keep adjusting until I "converge"? Also, my displacements are very strange, with the column squashing uniformly outward by a factor of roughly double my initial radius.
**When I switch the solver over the to I get a buckling factor of 0 only one mode is calculated. This happens even with a load double the calculated Euler buckling load. I'm not getting the weird squashing displacement like before, but the CCX output conclusion of "maybe no buckling occurs" doesn't tell me what I need to know. Or does it at least direct me one way or another?
Given the inconclusive results above I switched over to --Nonlinear Static 3D-- analysis:
**I couldn't get convergence with the , even when stepping my loads down to 0.75x, 0.50x, and 0.25xFcr. When I stopped the analysis at least the displaced shape looked good.
**Moving on to the solver I selected automatic time stepping, as recommended in the Mecway manual. At 1.00x Fcr I do not get a convergence. At 0.97xFcr I get a convergence and a lateral deflection that makes sense just before buckling. At 0.98xFcr I again am not converging. This seems to indicate that buckling occurs somewhere around the 0.97x mark. In analyzing my hole in the light pole I would narrow this down further by recording max deflections at say 0.93x, 0.94x, 0.95x and 0.96x Fcr to see where the displacement begins to accelerate. Is this how I should be using the nonlinear analysis to check buckling? Is there a more automated approach that I'm missing. I'm not seeing displacements in the CCX output file, only the incremental displacement. And I'm not even sure what units are being used in the CCX output file.
0.97xFcr seems reasonable considering the inherent error in FEA approximation and the mesh size I chose. In this case my moment of inertia of the FEA section is very close to 0.95 of the fully round section.
Sorry for the long start to the discussion, but I was hoping to be clear and thorough. I appreciate your input.
Note: The attached file has a vertical load input of 0.97x the Euler buckling load (Fcr). I listed all numerical values below as percentages of Fcr to avoid anyone having to do any unit conversions to understand what I'm saying.
I am using hex8 elements so that I can try both Buckling3D and Nonlinear Static 3D analyses. I have rigid plates on each end of the tube with pinned constraints and a concentrated vertical load applied to the center of the top plate. To initiate buckling I have placed a small horizontal near the midpoint of the column. If you want to skip the seemingly inconclusive tests, go to the last "**" below.
I started first with a --Buckling3D-- analysis:
**Using the I'm not sure what shift point to use. The warning that appears when you have the shift point at "0" says to set the shift point to a value between zero and the lowest buckling factor. But whatever shift point I input seems to be very close to the buckling factor listed in the results and all of my buckling factors are within 1% of each other. Do I need to start at a high shift point and keep adjusting until I "converge"? Also, my displacements are very strange, with the column squashing uniformly outward by a factor of roughly double my initial radius.
**When I switch the solver over the to I get a buckling factor of 0 only one mode is calculated. This happens even with a load double the calculated Euler buckling load. I'm not getting the weird squashing displacement like before, but the CCX output conclusion of "maybe no buckling occurs" doesn't tell me what I need to know. Or does it at least direct me one way or another?
Given the inconclusive results above I switched over to --Nonlinear Static 3D-- analysis:
**I couldn't get convergence with the , even when stepping my loads down to 0.75x, 0.50x, and 0.25xFcr. When I stopped the analysis at least the displaced shape looked good.
**Moving on to the solver I selected automatic time stepping, as recommended in the Mecway manual. At 1.00x Fcr I do not get a convergence. At 0.97xFcr I get a convergence and a lateral deflection that makes sense just before buckling. At 0.98xFcr I again am not converging. This seems to indicate that buckling occurs somewhere around the 0.97x mark. In analyzing my hole in the light pole I would narrow this down further by recording max deflections at say 0.93x, 0.94x, 0.95x and 0.96x Fcr to see where the displacement begins to accelerate. Is this how I should be using the nonlinear analysis to check buckling? Is there a more automated approach that I'm missing. I'm not seeing displacements in the CCX output file, only the incremental displacement. And I'm not even sure what units are being used in the CCX output file.
0.97xFcr seems reasonable considering the inherent error in FEA approximation and the mesh size I chose. In this case my moment of inertia of the FEA section is very close to 0.95 of the fully round section.
Sorry for the long start to the discussion, but I was hoping to be clear and thorough. I appreciate your input.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
**1) The displacement for the first few modes shows rigid body rotation which looks like radial expansion/contraction with the large automatic deformation scaling factor. To prevent these modes appearing, constrain an off-axis node in the X (for a node on the YZ plane) or Z (for a node on the YX plane) direction. Then you find the lowest buckling factor stays at 1. I normally only change the shift point in powers of 10, so using 0.1 for this is OK. If you orders of magnitude lower, you see error appearing in the 1st buckling factor.
**2) Same cause as **1)
**3) Same cause as **1)
**4) The easier way is to use time steps:
Mecway always runs CCX using m,kg,s units and automatically converts to whatever you choose when it imports the solution. So if you're looking at its output files directly, they'll be in those units.
For some reason whenever you identified a solver in your post, the word didn't appear, like "Moving on to the solver I selected". Did you use special formatting or something? This forum software is a bit flakey and it might have quietly deleted something.
Thank you so much for the useful comments and quick response! That is exactly what I needed (and was hoping for with the time stepping).
I was trying to make the solver labels stand out by adding two minus symbols in from and back. I will just use the bold and italic formatting from now on.
For the sake of reference by others, the Analysis method and Solver for each trial are as follows:
Is it possible to peek at your Analysis Settings window on your Non-Linear Static 3D solution.
I've input your suggested values but I'm not getting the expected solution. My time step graphs are do not look smooth like yours, and when I decrease the time step, the solver won't converge.
~CWharPE
A few tips:
1) I find it easier to set a unit load for linear buckling, because the "buckling factor" then tells you the buckling load directly, ie it is a multiple of the unit load you applied.
2) When you do non-linear buckling try to use displacement controlled loading if you can, ie impose a fixed displacement to a node instead of a force and measure its reaction load.
3) Buckling is sensitive to initial imperfections. If you are doing non-linear buckling you need to perturb the initial nominal geometry with imperfections, usually coming from the vibration modes.
I'm not sure how to do this with Mecway/CCX, but might have a look at this tonight and report back here.This looks like it is done via the 'PERTURBATION' parameter on the *STEP keyword.4) To interpret the non-linear buckling analysis you need to plot the load vs deflection, and you are looking for the point where the deflections start to increase disproportionately to the load. In the past I've either decided this by eye or come up with an offset tangent curve or something like that to decide where this 'buckling point' is.
Pete.
Another point of the exercise was to see how close to theory the results came. For quick comparison, I am using the calculator found here: https://amesweb.info/Beam/Column-Buckling-Calculator.aspx.
Like Pete, I'm trying to figure out where the break-point is on these plots (post-it notes taped to my display along tangents, etc.). Is there a more definitive method I am missing?
@badbunny Do you have a simple example I could follow with displacement controlled loading? Thanks.