Make sure that there are no differences in settings such as load, material model, and so on. If you can’t use the same mesh (generated in the same preprocessor) for all analyses then try to recreate it as accurately as possible (take a closer look at local refinements if you use those). If you still get slightly different results then it’s probably due to differences in formulations and algorithms used in each of these programs. It’s very common that there are some small discrepancies in results when comparing various solvers.

How the direction of the load is defined as the member deforms may also be relevant.

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

Doug Jenkins
Interactive Design Services
http://newtonexcelbach.wordpress.com/

I have seen this, too, with absolutely identical models between ABAQUS and ANSYS. The eigenvalue buckling results are different between the two software. I took extreme precautions to ensure that the models were identical.

Different element formulations. Different eigensolvers. Both are approximations.

Have all 3 solutions converged though? There will be discrepancies when the model is not converged, but I would expect those them to decrease once the model has reached convergence.

Brian
www.espcomposites.com

@All. Thank you. I believe it has something to do with the iteration schemes and contact between the skirt and the vessel. In Ansys, one must manually define the contact edges while Nei Inventor Nastran creates a continuous, conformal mesh that does not need contact definition. SW has triangular elements (so I'm leaving it out of the discussion), others have 8-node quads. Beyond that all models were set up with identical material, mesh size and BCs. However, I do not know how to interpret the buckling load factor showing ~ 20-30% difference.

If you plot the lowest buckling mode shape in each analysis application with an exaggerated amplitude (and / or colour contour and animation), you will be able to compare the mode shapes that are computed. You may find for example that subtle differences in applied support boundary conditions (simple support vs fully fixed) can change the buckling mode shape and load factor significantly. When all analysis packages show the same buckling mode shape, you would expect the buckling load factors to be very similar.

http://julianh72.blogspot.com

Could you post full details of the model and loading? I'd like to see what I get with different software.

Doug Jenkins
Interactive Design Services
http://newtonexcelbach.wordpress.com/

@ IDS, its ASME PTB-3 example 5.4.

From ASME PTB-3

Quote:

Evaluate the following tower, Figure E5.4-1, for compliance with respect to the Type-1 buckling criteria provided in paragraph 5.4.1.2.

• Material – Shell and Heads = SA-516, Grade 70, Normalized
• Design Conditions = -14.7 psig at 300oF
• Corrosion Allowance = 0.125 inches

Attached: STEP file.

• https://files.engineering.com/getfile.aspx?folder=099695ec-8165-469c-9fa1-8

there seems to be something wrong with your download link for the STEP file. I'm not able to download. Can you check and re-upload from your side?

and what of element size ? type ??

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

rb1957, CQUAD8 elements, various sizes, starting from 4"

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

• https://files.engineering.com/getfile.aspx?folder=8a1dfce8-9f96-4b43-9fe3-8

I wonder if the solution is from an ANSYS FEA and no one looked at other codes ?

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 ?

Okay.

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.

@nlgyro, thanks for taking a look. The mode shapes are probably going to be the same. I assumed that the PTB-3 is close to a benchmark, but there appears to be a lot of errors in the 2013 edition.

Searching for Type-1 buckling criteria, I found:
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/

Did the analysis using cquad8 elements with an element size of 2.5 inches. The lowest eigenvalue is 10.902 (10.918 using 4-noded elements of 2.5in size). The procedure is the same. Attached is the mode-shape corresponding to the lowest eigenvalue.



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.

I was able to get some computing time at a local university over the weekend that uses Inventor Nastran 2020.
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.

@nlgyro Thank you for taking a detailed look at the problem. FEMAP, too, predicted a linear buckling load factor that was closer to ANSYS (linear). There's certainly something dubious about Inventor Nastran. Also, the book you referred to is 'Buckling of Thin Shells' by JM Rotter/Teng?

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.

Yes that's the book. Also available on on Amazon at:

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!!

I think I found out the reason why Inventor Nastran is so off on the buckling load factors.

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!!

@nlgyro,

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.

The follower force effects for linear solutions were added into MSC.Nastran some 25 years back. NX.Nastran started its life as MSC.Nastran v2001 (which by then has follower force effects included into SOL 105) and built thereon. Inventor nastran which was earlier NEi nastran started with the initial nastran level 16 (I assume) and took a different route. But it's pretty clear this capability was never added by Noran Engineering.