Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Simcenter Nastran Forum
- Re: Non linear analysis with sequential loads

Options

- Start Article
- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-14-2019 06:44 AM

Hi Alberto,

thank you very much. Now i know how sol601 works. I did the setup you described and defined force to apply at 5seconds. The pressure is applied to reach the maximum at 4 seconds.

If i run the job only with pressure it convergences. But with the setup described below the job begins to not convergence at exactly 5 seconds where the force is added.

Do you have a tip for me?

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-14-2019 07:17 AM - edited 01-14-2019 07:18 AM

@PuddingBaer91, can you share the model?

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-14-2019 07:46 AM

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-14-2019 12:36 PM

Thank you @Karachun for your clarification.

My suggesion to @PuddingBaer91 was focused on *"SOL601,106 Advanced Nonlinear Static"* solution and not on *"SOL601,126 Advanced Nonlinear Transient"*. I modified my previous posts in order to be clearer.

For this reason I tell that in "*SOL601,106 Advanced Nonlinear Static" *the time is fictitous: this is a static solution (not a transient solution like instead *"SOL601,126 Advanced Nonlinear Transient"* or maybe "SOL701").

If I understood well, for this problem a static (non-linear) solution is enought.

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-14-2019 03:32 PM - edited 01-14-2019 03:33 PM

Yes, this is right. Also in SOL 601,106 you can enable "fake dynamics", solver use inertia terms. This can help when you model postbuckling or other cases where stiffness matrix can become singular at some timestep.

Here is screenshot from Femap, maybe in NX setting will be similar.

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-15-2019 05:47 AM

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-15-2019 11:56 AM

Can you post mesh and analysis setting in .dat or .bdf format (I already export model at work and copy to USB flash drive but forgot usb flash itself)?

BTW can you tell what results you want to obtain from this simulation? You already tell how you want to perform simulation, but not tell why (obtain max tangential force when bricks don’t slide or you want to study behavior of whole structure). Answer to this question can give you the right way to solve model.

Highlighted

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-15-2019 03:51 PM - edited 01-16-2019 05:41 AM

Dear @PuddingBaer91, below you can find the file of the model debugged.

Here some notes:

- The main problem can be easily found by hands.

You specify a max load of F_external=15'000 N.

Hence the friction force is F_mu=F_normal*mu=pressure*area*mu=750mm^2*50MPa*0.18 = 6'750 N.

Hence the overall force pushing on the spring is F_spring = F_external-F_mu = 8250 N.

The problem is here. The axial stiffness of the spring is 100 N/mm, hence you get a displacement of dx=F/K=8250/100 =**82.5 mm**. Note that your plates are**50 mm**long, hence the problem can not statically solved because the plate will deattach!!*Note: during the force loading, the contact area will decrease because the lower body move towards the spring hence you get a***non-linearity that tends to reduce the friction force**. The previous calculation is based on a simple case where there is not lower body movment. In the real sistem the spring is compressed much more than 82.5 mm due to a reduced friction force. This problem does not concern to NX Nastran but to the phisics of the problem: with those parameters you can not obtain reasonable results.According to that I increased of x50 the stiffness of the spring from 100 N/mm to 5000 N/mm.

As we aspected, the theoretical displacement is now 1.65 mm (underestimation because we do not keep into account of the reduction of friction force), while NX Nastran give about 2.1 mm. Hence reasonable results - In "Case Control" -> "Strategy Parameters" -> "Equilibrium" I set LSEARCH = YES and MAXITE = 50. That help a lot the solving method. Expert users will help you to understand this point.

- In "Case Control" -> "Output Request", consider to remove from results the stress results if you are just inreested into them (eg non linear stress are not interesting for this analysis). This is only a waste of time!
- Very important: in "Parameter", click on "Large Displacement" to keep into account the strong geometrical non-linearity (large strain flag is not required since your material is linear).
- Just for my convention I modified the time from 0 to 1 (this is not an error but my habit).
- I modified the ratio between the iteration calculated for the pressiore loading (0<=t<=0.3 s) and the force loading (0.3<=t<=1 s). Basically I the pressure loading is less critical then force loading. Hence we spend higher number of iteration (70%) for force loading. This choice is assuemed becuase I think that the pressure loading do not lead to non-linearity (you can also solve by hands) but the force loading is a strongly non-linear phenomena due to the reduction of friction force (see point 1) and for this reason require higher number of iterations than pressure.
- I think that you boundary conditions are not fully correct. The bodies slightly rotate along Z axis! Please take care about Boundary Condition of your model!!

In my case now the simulation take about 600 interations (I think 30-40 min on my laptop, but the computational time depends on hardware resources).

This is caused by the contact of the upper part that is bended under the pressure loading.

Here is the picture of the final step:

I hope that can help you.

Regards,

A

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-16-2019 07:14 AM

Hey Alberto,

THANK YOU VERY MUCH FOR YOUR ENGAGED HELP

I owe you an apology. Because i can't share the real model i have done a quick and dirty representation model with all the errors you explained... sorry

In real model i model only a sector to save ressources. Because of 100 trys to get it working a really made the mistake and didn't divided the force through the sector count. So now it works I also like your tips.

So my problem is now solved

Thank you very much Alberto

Re: Non linear analysis with sequential loads

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

02-25-2019 05:58 AM

Cyril

Follow Siemens PLM Software

© 2019 Siemens Product Lifecycle Management Software Inc