## Different Buckling load Factors for Same Model, Different Software

## Different Buckling load Factors for Same Model, Different Software

(OP)

Hi,

I'm practicing the ASME PTB-3 example 5.4. I get different values of the buckling load factor for the model (8 node shell elements). Any hints as to why this is happening?

Nei Nastran Inventor = 14.655

Solidworks = 15.587

Ansys Workbench = 11.954 (matches PTB-3 Result, minus the load factor)

Thank you

I'm practicing the ASME PTB-3 example 5.4. I get different values of the buckling load factor for the model (8 node shell elements). Any hints as to why this is happening?

Nei Nastran Inventor = 14.655

Solidworks = 15.587

Ansys Workbench = 11.954 (matches PTB-3 Result, minus the load factor)

Thank you

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

https://newtonexcelbach.com/2011/01/01/buckling-of...

Doug Jenkins

Interactive Design Services

http://newtonexcelbach.wordpress.com/

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

Brian

www.espcomposites.com

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

http://julianh72.blogspot.com

## RE: Different Buckling load Factors for Same Model, Different Software

Doug Jenkins

Interactive Design Services

http://newtonexcelbach.wordpress.com/

## RE: Different Buckling load Factors for Same Model, Different Software

From ASME PTB-3

Attached: STEP file.

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

another day in paradise, or is paradise one day closer ?

## RE: Different Buckling load Factors for Same Model, Different Software

Also attached updated file (doesn't like the '+' symbol in the name)

## RE: Different Buckling load Factors for Same Model, Different Software

Do the mode shapes look similar ?

Is there a "right" hand book solution ? Are we talking about buckling of an unpressurised cylinder ?

4" element size is small compared to the tank dimensions, but not that small compared to the thickness (1.125").

I wonder about 20 node Brick 3D elements ?

another day in paradise, or is paradise one day closer ?

## RE: Different Buckling load Factors for Same Model, Different Software

I have some first pass results done using MSC.Nastran. Used a 4-noded cquad4 shell element of size 2.5inches for a linear buckling analysis. Per the ASME example the static pressure load is treated as a pre-load for the buckling case and the buckling factors are calc'ed. The lowest eigenvalue (buckling load factor) is 10.918. I don't think the results using a cquad8 would be that different, but I'll give it a stab tomorrow (it's already past midnight my time!!). Here attached to this post is the mode-shape corresponding to the lowest eigenvalue.

## RE: Different Buckling load Factors for Same Model, Different Software

## RE: Different Buckling load Factors for Same Model, Different Software

https://becht.com/becht-blog/entry/basics-of-desig...

which doesn't actually answer the original question, but seems to have a lot of good advice relevant to this sort of analysis.

Doug Jenkins

Interactive Design Services

http://newtonexcelbach.wordpress.com/

## RE: Different Buckling load Factors for Same Model, Different Software

The static preload (obviously) has a big influence on the analysis. Without the use of preload and doing a regular linear buckling analysis the lowest eigenvalue is 11.902 which closely matches your ANSYS results (11.954). ASME ptb-3 (2013 edition) treats the external pressure load as a preloads to calc the buckling factor and thats what precisely been done in my models. I obviously can't vouch for the veracity of the 2013 edition as this is not something I use for my field of work day-in and day-out!! The mode-shapes that I have plotted above are identical to the shapes given in ASME ptb-3.

Coming back to you original question. You did mention contacts in your ANSYS model. Are you running it non-linear?? Or is your ANSYS run just a linear buckling analysis??Are you defining external pressure load as a static preload in your models across all packages you have used?? Are you sure that 8-noded shell is supported in a buckling analysis for inventor nastran?? You have discounted the SW results on account of its use of trias, so when compared with inventor nastran and the difference that you vis-a-vis ANSYS your answers to the above questions could provide some insight.

## RE: Different Buckling load Factors for Same Model, Different Software

To check the validity of the code for buckling I took a problem that can be hand calc'ed.

I took the same example as your ASME pressure vessel, removed the elliptical heads replaced them with flat end-plates, and removed the skirt.

So essentially the model is a cylinder with flat end-plates. I loaded it with an overall external pressure and used a 'classical' simple support condition at the ends.

Steel is used as the material.

The critical buckling stress is provided in Rotter's text chapter 5 eq(8)

Here is the summary of the hand-calc

E = 2.90E+07 psi

nu = 0.3

t = 1.125 in

r = 45.563 in

L = 636 in

Z = 7527.918

L/r = 13.959

Scr = 6407.300 psi

Pcr = 158.205 psi

Modeled the problem in both MSC.Nastran and Autodesk Nastran using 4-noded CQUAD4 shell elements of element size 2.5 inches.

Ran a linear buckling analysis and here are the results:

Pcr (Theory) = 158.205 psi

Pcr(MSC.Nastran) = 159.870 psi

Pcr (Inventor) = 211.120 psi

% difference Pcr(FEA) / Pcr(Theory)

MSC.Nastran = +1%

Inventor Nastran = +33%

So there is your +30% that you were talking about in your earlier posts. For a simple test problem Inventor over-estimates the buckling pressure/stress by +30%.

The static analysis b/w both codes are identical. Peak deflection is at the flat end-plates. Both codes register 0.022in as the peak deflection under 1psi pressure.

So there is something going wrong in the buckling solution in Inventor. Maybe the differential stiffness formulation is a suspect or the implementation of eigenvalue solver

is a suspect. But if I were you I would junk this code as it can't predict a classical hand calc'ed problem!

I don't have access to ANSYS but it’s a well respected code in the industry so I wouldn't expect it to misbehave for such problems.

## RE: Different Buckling load Factors for Same Model, Different Software

If I use linear buckling to iterate two loads (one constant prestress and the other variable perturbation) to get a buckling load factor of 1 based on the image below, Inventor Nastran is around 13% off the Ansys solution.

## RE: Different Buckling load Factors for Same Model, Different Software

https://www.amazon.com/Buckling-Thin-Metal-Shells-...

I've never been a fan of CAD integrated FE solvers primary because they just aim for quick & dirty. But when you have something that is off by ~30% for a test case it's just BS!!

## RE: Different Buckling load Factors for Same Model, Different Software

Its because the solver does not include the effects of follower force for pressure loads into the linear buckling solutions. For a loading which is not constant, but changes with the shape or orientation of the elements (structure supporting pressure loads), the displacement dependent loads (called the follower force term) needs to be computed. The follower force vector is formed for each dof in the model and appended to form the follower force matrix.

By default MSC and NX flavors of Nastran calculate this and include it with the differential stiffness, but Inventor Nastran does not.

I ran the above mentioned test problem with the MSC.Nastran with the effects of the follower force switched off for the linear buckling solution and the results match those of Inventor Nastran to less than 1% but are off from theory by the ~+30%.

So the calculation and the inclusion of the follower force matrix for loads which change with the shape and the orientation of the element in the linear buckling solution is important and the absence of this causes errors. The results from Inventor Nastran for the above mentioned test problem are an example of this.

Another example which can be illustrated (which has been discussed at length on this forum) is this:

Link

Let us take a test case as shown below:

(Note: All values given above are in SI)

Per Roarks the buckling pressure is given as:

qcr = 3*E*I/R^3 = 1.74E+05 N/m

Doing a linear buckling analysis in MSC.Nastran:

qcr = 1.71E+05 N/m

So the results match theory to ~2%

Doing a linear buckling analysis in Inventor Nastran:

qcr = 2.09E+05 N/m

The results are off theory by ~20%

It looks like Inventor Nastran would require the user to do a full fledged geometric non-linear analysis to compute the buckling load. This would include the follower force effects. But doing this for a linear problem just because the linear buckling solution fails to include the follower force terms sounds to me like a huge over-kill!!

## RE: Different Buckling load Factors for Same Model, Different Software

Thank you for taking a deep dive into this. I find it strange because Inventor is using the same Nastran SOL 105 solver for linear buckling.

## RE: Different Buckling load Factors for Same Model, Different Software