Load Cases for Non Linear Analysis

[patolon]

Hello everybody,

I would like to run a non linear static to account for large displacements. The pressure load to apply has a large magnitude so I would like to create a sort of break down by having incremental loading.

Is it possible in femap to do that? I guess I can create several load sets, but then how can I apply these gradually, or step by step?

Thanks a lot for your comments on this topic!

Pat

 

[Wnuczko]

Hi,

You have two options.

1. Go to Analyses > Nonlinear > Edit > Click Next until you reach Nonlinear Control Options > Set Time Steps (ex.100) > Set Time increment (ex. 0,01). > Output Controll (if needed) > 3..ALL
2. Create ramp function vs. Time. and use it in your pressure definition.

Acc to my knowledge both ways will work the same. But I'm new to Femap.

I hope this helps,
W.

 

[ThomasH]

Hi

Since the loading is static, go to "Nastran Nonlinear - Control Options". There you will find "Increments or Time Steps", say you select 10. "Time Increments will be unavailable since it is statics. Fopr output Control you can select Yes.

What happens when selecting 10 is that you will get results for 10% loading, 20% loading and so on up to 100%.

You can also "play" with incremental load sets and so on. If you want to know how that is done, let me know.

Good luck

Thomas

 

[patolon]

Hello,

Thanks for these replies!

Instead of creating a ramp load via the function, what if I create subcases and create multiset in the analysis deck?

For example let's say I ve got a 100 bar pressure load. I create 3 load cases, 10, 50 and 100 bar.
Then, I have 'none' in the the load in the analysis menu, and instead I have case1 case2 and case3 in the multiset.

What will femap do? Run a non linear static for each one, or consider each case as the load step?

Not sure I fully understand how the multiset section works with femap!

Thanks for your support!

 

[ThomasH]

Hi

Which solver are you using (MSC/NX/NEi(Autodesk)?

Thomas

 

[patolon]

I m using Nastran!

 

[ThomasH]

Yes, I understand that you use Nastran. But what "flavor" more exact? How things work are to some extent solver dependent.

Thomas

 

[ThomasH]

Hi again

Let me explain this in another way. Since you describe it the way you do I assume that you use NX Nastran integrated in Femap.

Say that you have three load cases and connect them to three subcases: Case 1 (10 bar), Case 2 (50 bar) and Case 3 (100 bar).

What Nastran will do is for the first case increase to load form 0 to 10 in the number of increments that you have selected, in Case 2 it will increase the load from 10 to 50 and in case three from 50 to 100.

Between the subcases you can change not only the loading but the support conditions and/or the solver settings. Since the loading path can effect the result this approach can be very effecient.

This description applies to, as far as i know, the threes versions MSC/NX/NEi. The reason I asked what version you use is that in NEi(Autodesk) there is a parameter "nlsubcreinit". That parameter gives you an option to instead of loading 0-10-50-100 you can use 0-10, 0-50, 0-100. The subcases are analyzed independent of each other. I don't think this option is available in MSC or NX.

Best Regards

Thomas