Nonlinear Static analysis failed 10 times

[Anonymous]

Hello folks,

I am trying to analyze pipe under external pressure which is applied inside the weldolet connection. I defined the nonlinear material and wana see stress as per ASME Section VIII Div 2.

I setup the nonlinear static analysis and tried about 10 times and it failed/crashed.

It is running smooth until few iterations and then it switched to "Subiterations" and this is where it took a lot of time and then crashed.

I am attaching the files, so if any of you on this forum can help me plz. Model is defined fully, i.e., geometry, BCs, loadings, material (non-linear one 'Plastic option' stress-strain curve [attached as well]), meshing, Surface Contacts (as this is welded so all contacts are bonded). All files are in zip file.

I am using Inventor 2018 with Nastran In Cad on Windows 10 64 bit OS.

Thanks

[John_Holtz]

Hi @Anonymous

I do not know if the following is causing a problem, but it certainly is not helping. There is considerable interference between the weld and both the header (shell) and weldolet. Here is an image with a 1/4 section view. (The problem with interferences and contact is that the elements are adjusted to eliminate the interference. This could create distorted elements.)

Figure 1. Interference with weld

If it still does not converge, here are my suggestions:

• Try using a convergence of displacement and load, or displacement and work. I do not suggest running the analysis without using the displacement criteria.
• The transition from elastic material to plastic material can be difficult to converge when there is a rapid change. (The modulus of elasticity is 2.9E7 psi. The first segment after the yield stress has a modulus of 1.76E5 psi. Thanks for the spreadsheet :-). Imagine adding a fillet between those segment and splitting the fillet into 10 points. That will give a smoother transition from elastic to plastic. Then during the analysis, you want to have sufficient number of load increments so that one step does not jump over half of those segments! (Instead of using 1 subcase, you can use 2 subcases. Subcase 1 ramps the load to 95% of yield with a few load increments, and subcase 2 ramps to 100% load with many more load increments.)

Let me know if you have any questions.

[Anonymous]

Thanks John for pointing out interference issue. I certainly missed that. Now I fixed that problem.

Right now I am running the analysis with "displacement and work" convergence criteria using default tolerances.  I added about 50 Load Increments and fine meshed the weld between the pipe and weld-o-let.

I just used only one Subcase as I don't know how to define various Subcases. If you please point some helpful link, I would appreciate that.

Attached is the model for information. I will keep posting about any progress 🙂 or failure :(.

Thanks,

[Anonymous]

Another question, once non-linear enters into "Subincrement" stage for solving, then how many Subincrements are there for that increment.

Thanks,

[shigeaki.k]

Hello @Anonymous,

it depends. There is the setting for number of iterations before the increment is bisected. This number changes from 40 to higher near convergence. See comment 5 in the Autodesk Nastran help documentation for NLPARM.  If you are wondering what the ideal number should be, there isn't really a fixed answer. I tend to try to set the number of increments so that convergence for a subincrement is achieved within 20~30 iterations, but this is not always the case.

Regards,

Shigeaki K.

[John_Holtz · Accepted solution]

Hi,

Here is a brief explanation of the subcases.

• Although the analysis is static, you can think of the subcases and increments as "time steps".
• Different subcases are used to change the size of the time steps, or to see what happens when the load changes from one value to another, or to see what happens when additional loads are added or existing loads are removed.
• In your current model, under the "Subcases" branch of the model tree, there is "Subcase 2". Subcase 2 includes the Nonlinear Setup 1, Loads 1, 2, 3, Constraint 3, Results, and so on.
• You can right-click on the "Subcases" branch and create a new subcase. Let's call it "Subcase 3", and it will include Nonlinear Setup 2, Loads, Constraints, and so on.
• Technically, all of the branches can change from one subcase to the next. So for the nonlinear setup, you might want to use 10 steps for the first subcase, and then 50 steps in the next subcase (assuming that the model becomes more difficult to converge during the second subcase).
• Usually, you use the same constraints in all of the subcases. (When you create a new subcase, you can choose right then which loads and constraints you want to include).
• Usually, you have different loads in the subcases so that you can see what happens when the load changes from A to B.

So for your model, you might setup the subcases as follows where the primary purpose is to progress quickly through the range where the material is linear, and then proceed more slowly as the material yields. (I am just pulling numbers out of the air; I have not progressed through your model far enough to know when things change.)

	Subcase 2	Subcase 3
Purpose	Load the model up to 95% of the yield stress. (Let’s assume that corresponds to 70% of max load)	Load the model to the full load.
Nonlinear Setup > Number of Increments	10 (assuming that it converges easily in the linear range of the material)	50 (assuming it requires more steps to converge when it goes plastic)
Load 1	0.7*Load 1	1.0*Load 1
Load 2	0.7*Load 2	1.0*Load 2
Load 3	0.7*Load 3	1.0*Load 3
Constraint 3	Constraints on the ends	Same constraints

I will let you know what I find out about your model and the convergence.

[Anonymous]

Thanks @John_Holtz and @shigeaki.k.

Hi @John_Holtz,

Thanks for sharing the info to setup subcases. I tried and analysis is going on one of my machine. The other analysis is still going on my remote machine and it is about 17 hrs now since I started that analysis.

I would like to share results from Simulation Mechanical with the same model and it did converge and took 7.5 hrs. The model buckle at 40% of load. Please see attached pics.

Nastran In-Cad analysis seems not converging at this load. Thoughts?

Thanks,

[Anonymous]

[John_Holtz]

Hi @Anonymous

If the model really buckles, that could be the problem with the static stress analysis in In-CAD. It is difficult for a static analysis to get through any type of buckling where the stiffness instantaneously transitions from one state to another. (I assume that you used MES in Simulation Mechanical, so the mass helps with the transition from one state through buckling to the other state.)

I read somewhere that the "Arc Length" method can be used for models that have snap-through behavior. The Arc Length method is set under the Nonlinear Setup. (I was either reading this Nonlinear Setup page, or something else that I cannot find at the moment.)

[Anonymous]

Hi @John_Holtz,

Yes, I used MES in Simulation Mechanical.

Now running with Arc Length method active. Hope that this helps.

Cheers,

[Anonymous]

Hi @John_Holtz and fellow members:

Its been 30 hrs that analysis is still going on. Analysis went to "Sub-increment" and it is keep going. Below are snapshots at various sub-iterations levels:

Here are settings that I used. I used Arc Length method as well.

Any suggestions ?

Thanks,

[John_Holtz]

Hi @Anonymous 

Since it seems that the model is buckling, I tried a "Nonlinear Buckling" analysis. It got as far as 44.54% load before it failed to converge. Here is a plot of the displacement. 

Have you tried a nonlinear transient analysis? I am thinking that the Simulation Mechanical MES analysis may have converged better because of the inertia. As you can see, the displacement (and therefore the stiffness) is changing quite rapidly, and that may be too much for a static solution. (Or the difference could have been the nonlinear stiffness update method; that is, full Newton-Raphson versus modified Newton-Raphson.) I think that limiting the number of sub-increments will not help -- other than to cause the analysis to fail sooner.

I do not know if we have asked this question or not. Do you need to see what happens after the pipe buckles? In other words, you are trying to find more than just the load at which it buckles.

[John_Holtz]

Hi @Anonymous 

I wanted to follow-up with you to see if you have made any progress on this analysis and/or have any questions.