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
- 3D Simulation - Femap Forum
- Duration of advanced non linear Analysis

Options

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

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

08-30-2015 09:48 PM

Hello,

I´m doing Analysis with the SOL601 currently and it seems to need very long.

My model has something like 10700 Elements and I´m doing an analysis with 1000 steps, a time increment of 0,001 and 15 increments on each step .... after 13 hours the analysis ended on step 582 with a time of 0,6025 so far , because it cant get the convergence anymore.

Is it normal , that it takes so long ?

How can I get sure, to avoid convergence errors ?

Is it advisable to decrease the number of increments on each step or will it influence the results to much ?

Is there maybe a tolerance value which I can regulate in the right way ?

The default solver is "direct sparse" is this the right solver for large displacement analysis ?

I would be very thankful for any answers or tips.

Greets

8 REPLIES

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

09-01-2015 05:22 AM

Hello!,

Well, without the FEMAP model in hand is quite difficult to see the reason of the lack of convergence, things in general are really complex in nonlinear analysis. Take a look to Advanced Nonlinear manual, read in detail, is the best source of information, quite complete and useful.

Here you are a few recommendations, I suggest to identify sources of nonlinearity and reduce them until solution converges (of course, an initial SOL101 run should be done to see the level of displacements and stress results!!):

**• For geometric nonlinearity:**

- Use small strain instead of large strain (LGSTRN).
- Use small displacement instead of large displacement (LGDISP).

**• For material nonlinearity:**

- Extend material curves to avoid element rupture (XTCURVE).

**• For load nonlinearity:**

- Use deformation independent loading (LOADOPT).
- Apply loads more gradually.

**• For contact nonlinearity:**

- Add or remove friction.
- Use small displacement contact instead of large displacement contact (CTDISP).
- Add contact compliance (CFACTOR1).
- Increase friction regularization parameter (EPST).
- Gradually remove initial penetrations (INIPENE/TZPENE).

Regarding loads & boundary conditions, I suggest to use prescribed displacements instead of forces where possible.

The causes of diverging solution could be many, you may have rigid body modes (model is unstable), buckling occurs, contact separates, etc.. In general **the remedy is to allow more iterations, use deformation independent loads, or use smaller time steps**.

Also, if Automatic Time Stepping failed (ATS scheme used in AUTO INCREMENT=1), then change to the following method in the NXSTRAT Iteration & Convergence Parameters window:

**Use AUTO INCREMENT = 3 (TOTAL LOAD TLA Scheme).****Solver ignores any defined time steps and time functions.****Solver uses 50 steps of 0.2 seconds (TLANSTP).****All loads are scaled from 0 at t=0 to 100% at t=10.****MAXITE = 30 (TLAMXIT).****ATSSUBD = 64.****LSEARCH = 1.****MAXDISP = 0.05 * (max model dimension).**

Regarding solvers, the DIRECT SPARSE solver is the best, not doubt, your model is not big (10700 elements is nothing!) then not need to switch to another solver.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

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

09-01-2015 02:18 PM

In addition to Blas' suggestions, if you have multiple cores in your machine, in the Analysis Set Manager, go to the "NASTRAN Executive and Solutions Options" and turn on Parallel Processing and enter the number of cores your machine has.

I have dual Xeon processors, 64GB of RAM and my machine is set up without Hyperthreading, I can run your model in under 9 minutes with 12 cores in use. (I think it's the same one that you sent for the post-processing question).

Mark.

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

09-01-2015 08:14 PM

@masherman Yes, it is the same model, but did you change the parameters or did you just run the existing analysis which I created there ? Because that one, which I created have just 100 steps and a increment time of 0,01 with just 5 iterations per step .... for this analysis my computer needs 20 minutes with one core so maybe this could be the reason for your rushing calculation?

Or did you the 1000 Steps with 15 Iterations per step and a increment time of 0,001 seconds ?

Because this would be really impressive ^^

PS.

Had you the same doubled set of results like me ?

Thank you for the help so far, I am currently trying to benefit from them

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

09-02-2015 09:12 PM

So,

I tried a dozen of different analyzes , but I dont get the satisfactory results.

The only method which seemed to run nearly to the end was the TLA Method, but it has other problems. First of all I will show the model and explain it a little bit, so the you can imagine what my goal is.

You can see, that the model consists of 5 parts.

The 3 long tendons which lays out of the center from the silicone body and are attached to a rigid disc on the top of the silicone body. The idea is, that I pull one of the tendons , which causes the body to bend like an arc. This model is 120mm long and about 22mm thick in diameter. The tendons have an E of 10N/mm² and the silicone an E of 1,95 N/mm². This is the result of the TLA method with 2% of a 50N load

And this is the result of the TLA method with 77% of a 50N load

As you can see the results do not act like they should ... the tendon is streched all the time from 0-77% but the body is bending just a tiny bit ... the whole force seem to just compress the body.

This is the way the bending should look more like ^

This are the configurations which I could use from your post

but, I couldnt find the parameters **MAXITE = 30 (TLAMXIT). and ****ATSSUBD = 64. **

where are they and do you think changing them will cause a big difference in the results ?

If it helps, I could send you the .modfem file ... just give me your email.

PS.

I want to figure out which forces are needed to bend the body up to 180° .... with the SOL101 the model just breaks and looks like this already at 30N

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

09-03-2015 03:26 AM

Dear Nemonekto,

1.- The first action I will do here is meshing with HEX8 elements, avoiding the use of TET10 elements: you will get an immediate benefit, with the same element size the model database will reduce in the number of nodes about 10 times!!. This is very important in nonlinear analysis with contact, the size matter!!.

2.- Next you will make sure to have the same mesh in the tendon & body, avoiding the interference & penetration of both meshes: the solution is to use HEX20 elements, but this increase the model size a lot, or the "trick" is to have exactly the same mesh (node location) in both parts. You need to learn how to mesh with HEX elements, is very important (crucial!!) in advanced nonlinear analysis with contact (SOL601) to use hexaedral elements, **the target is HEX20, and better HEX27 (activating ELCV=1 parameter in NXSTRAT).**

3.- Regarding the **TLA scheme**, is the solver who select internally the mentioned parameters, to learn more about it I suggest to read carefully the Advanced Nonlinear manual, you will learn a lot, is a jewel!!.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

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

09-06-2015 10:43 PM

I have revised the model, so that its more suitable for a homogeneous mesh. It looks now like this.

The mesh of the tendons, the body on the tip have the same orientation and size and the amount of elements is decreased to 3200, so the calculations are going quite fast.

Nevertheless, the TLA-S is giving still the same results (normal TLA does not work) ... it is succesfull , but the results are physically impossible and therefore worthless. I tried it often with the ATS Method but it ends everytime in convergence problems ... I´ve set the iterations per step to the maximum of 999 and this helped alot ... but not enough.

So are you sure that the TLA-method is the right solution for my problem ?

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

09-07-2015 12:53 PM

Addition: Everytime I start a analysis the program is showing me this sentence

"Contact group 1 has 290 initially penetrating contactor nodes".

Shouldnt be there no penetrating contactor nodes, if I meshed it the way you told me ?

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

09-10-2015 10:07 AM

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc