Plate Buckling Approach for Non-Uniform and/or Biaxial Loads

[stress_geek]

Hello,
        For a laminated rectangular plate (Unstiffened) with uniaxial compression (Nx) Hyperizer uses the general orthotropic equation to calculate the Nxcr. But in a case where a moment about z axis is applied on the edges then Nx would be non uniformaly distributed along the edges in order to obtain the proper resultant moment. Hypersizer assumes this as uniformly distributed along the edges and uses the classical buckling equation in calculating Nxcr. My question is: 1.) Isn't this approach too conservative?

2.) In the case of biaxial loading with Nx being positive and Ny being negative I understand that Nxcr is calculated taking into account the +ve Nx. But is the stress ratio Rx calculated based on the compressive stress in the Y direction i.e; Rx= Nxcr/Ny

Thanks

[Phil]

Hello,
        For a laminated rectangular plate (Unstiffened) with uniaxial compression (Nx) Hyperizer uses the general orthotropic equation to calculate the Nxcr. But in a case where a moment about z axis is applied on the edges then Nx would be non uniformaly distributed along the edges in order to obtain the proper resultant moment. Hypersizer assumes this as uniformly distributed along the edges and uses the classical buckling equation in calculating Nxcr. My question is: 1.) Isn't this approach too conservative?

For the first case you describe, assume that half the plate is in compression and half is in tension.  (see the attached image at the bottom of this post - you must be signed it to see it)

HyperSizer does two things. 

First, it averages just the compressive stress, therefore the tensile stress is ignored completely.  Also, the load applied is not the maximum compressive stress, but the average.

Second, it takes into account the fact that the buckling length should be adjusted such that only the compressive part of the panel should be included in the buckling length.  So if half of the panel is in compression and half in tension, then the buckling length should be modified to approximately one-half the entered buckling length.  To see this effect, generate a stress report with sample calculations for panel buckling, and look at the panel buckling sample calculation.  The adjusted buckling lengths should be presented. 

These two operations should give reasonable buckling results that will match a buckling analysis that takes the actual load gradient into account and not be over-conservative.

2.) In the case of biaxial loading with Nx being positive and Ny being negative I understand that Nxcr is calculated taking into account the +ve Nx. But is the stress ratio Rx calculated based on the compressive stress in the Y direction i.e; Rx= Nxcr/Ny

Thanks

HyperSizer doesn't really calculate the critical Nxcr directly, rather given the Nx and Ny load, it calculates the eigenvalue for buckling.  From the eigenvalue, you can get the critical Nx and Ny by multiplying Nx_cr = Eigv * Nx_applied; Ny_cr = Eigv * Ny_applied.

Example,

Nx_applied = +300
Ny_applied = -1000

Eigv = 1.3

Nx_critical = Eigv * Nx_applied = +300 * 1.3 = +390
Ny_critical = Eigv * Ny_applied = -1000 * 1.3 = -1300

So the critical buckling load is:
Nx = +390
Ny = -1300

Note:  The margin of safety reported on the Failure tab is:
MS = Eigv - 1

Please let me know if you need further clarification.

[stress_geek]

Thanks for your reply. For buckling of flat panel where the panel is subjected to non uniform compressive load (Nx-Bending+Direct Compression) and a uniform compressive load (Ny), I generated a report and the report contains the following data:
1.) Object load which is the average of all negative compressive load in x (Nx), y (Ny) direction and average of negative shear (Nxy)
2.) Based on the report it seems like it calculates the critical Nxcr using the general orthotropic equation in which the effect of Ny is taken into account
3.) Then it calculates the stress ratio Rx= Nxcr/Ny
4.) Finally the report lists the interaction equation used to calculate the margin of safety.

What you explained is true for curved panels i.e; the report shows that a eigen value is calculated and the margin is based on the calculated eigen value. But this is not true for flat panels.

On the other hand, looking at the image you attached it seems that hypersizer breaks the load into pure bending and direct compression in case of compression and tension load on one edge. But the report calculates the object load as noted in Point 1 above. Can you please clarify?

[Phil]

I did a test on my own and I see the confusion.  The Rb listed in the stress report is shown as

Rb = Nx / Nx, cr,

however in reality, it is using the Eigenvalue from the from the biaxial solution.  So you could look at it as the following:

If Ny is controlling

     Rb = Ny / Ny,cr

If Nx is controlling

     Rb = Nx / Nx,cr

In reality, the eigenvalue is

     Eigv = Ny,cr / Ny = Nx,cr / Nx

So

     Rb = 1 / Eigv

Hopefully that makes sense.  I think the documentation can be changed to reflect this.

This is actually easier to see if you turn on the biaxial and the shear margins in addition to the interaction margin.  By definition, both of these two margins should be higher than the interaction margin, so there should be no danger of one of them controlling instead of the interaction.  However, if you turn these two margins on, you will get details of how these two margins are calculated.   If you do this, then you can more easily see where the Nx and Nx,cr in the biaxial calculation comes from. When you only have the interaction margin turned on, the details for the biaxial or shear buckling are not presented in the stress report.

When you turn on the biaxial buckling, you should see the updated buckling lengths.

[garyjh]

Can you please clarify what the "entered buckling length" is. Is it the X & Y buckling spans in the sizing form buckling tab? Do these have to be changed manually or does hypersizer determine the edge length of the panel that is in compression? Is the average compression load applied to the full edge span by default?

[Phil]

Yes, the "entered buckling length" is the X and Y buckling span that is entered on the sizing form buckling tab.

When you import a finite element model, HyperSizer attempt to read the geometry of each component and determine on its own what the proper buckling lengths should be.  If the component has a simple shape (i.e. relatively rectangular and singly connected), it usually does a good job with this.  However, if the component shape is very complex (for example elements on either side of a wing or something like that), then sometimes, the buckling length that HyperSizer chooses is not appropriate.

Open your FEM in the HyperSizer graphics window and turn on buckling lengths on the left hand side (the icon looks like a set of cross-hairs).  You can select components and adjust their buckling lengths on the sizing form if they do not look to be correct.

One thing to realize about HyperSizer's buckling analysis is that it calculates buckling assuming uniform loads on a representative rectangular area.  Typically buckling waves go between hard points like frames or shape control members.  So, it is important to make sure that your analysis is using the correct buckling lengths in order to get accurate results.  Your buckling length can actually be larger or smaller than the actual component area.  For example, say a component is defined so that it spans multiple frames.  In this case, the buckling length should not be the component length, but rather should be the frame spacing.  HyperSizer cannot automatically determine this, but the user should change the buckling length manually to the frame spacing.

Finally, in the case where you have compression and tension in the same panel, HyperSizer reduces the buckling length so that it only covers the compressive portion of the panel.  This is done automatically by HyperSizer and the user does not have to change anything.  HyperSizer does a pretty good job of this in most cases, but sometimes it can be over conservative in the statistical loads analysis if the loads are varying wildly over a component.  In this case, it is usually the best practice to split the component up so that you don't have wildly varying loads within one component.

Let me know if this helps.

[garyjh]

This is a question with regards to the shear that is used when analysing a panel.

Currently I am analysing a panel with loads obtained from an FE model. The majority (60% of area) of the panel is under positive shear. The positive shear average, std deviation & peak is greater in magnitude than the negative shear average, std deviation & peak. Yet the design to loads uses the lower magnitude negative shear average & std deviation.

Normally I would use the greatest magnitude of average shear with the negative Nx & Ny. Why does hypersizer not do this? This may lead to critical positive shear loads being missed.

[Phil]

You are technically correct, there is a possibility that a load combination could be missed if you only combine the postive shear with the postive Nx/Ny and the negative shear with the negative Nx/Ny (which is what HyperSizer does now).

The best workaround that I can suggest right now is to break the component in question into two different components, one that is all in positive shear and one that is all in negative shear.  Then you will be ensured to get all of the loads accounted for.

Note that if all of the component is in Nx compression, then the software should use this average compressive Nx load for both the "tension" and the "compression" loop.  Then the value that is reported will be that corresponding to the lowest margin of safety.

In other words... lets say

Nx_compression = -1000
Nx_tension = 0

Nxy_negative = -400
Nxy_postive = +600

HyperSizer would then analyze the following:

1) Nx = -1000; Nxy = -400
2) Nx = -1000; Nxy = +600

And would return the minimum margin from these two conditions.

However, if part of the structure is in tension and part in compression

Nx_compression = -1000
Nx_tension = +500

Then HyperSizer would analyze the structure with the following conditions:

1) Nx = -1000; Nxy = -400
2) Nx = +500; Nxy = +600

So it would never catch what could be a worse case Nx = -1000, Nxy = +600...

To catch this, you would need to re-define your component so that you don't have the wide variation of load.

I hope this helps.

Phil