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 - NX Nastran Forum
- Dynamic force

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
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-02-2015 08:09 AM

I want to apply a dynamic force to a model. I'm using NX9 but I also have the availability of NX10.

My model is an assembly wich also contains surface-to-surface contact and gluing. I have added my simulation files to this post. In there you can see I have tried 3 solvers, all SOL101 linear.

__static force__: Force is constant with 420N__dynamic force__: I used a table to define the force (0,1 / 0.01,200 / 0.02,350 / 0.03,400 / 0.04,420 / 0.05,400 / 0.06,360 / 0.07,320 / 0.08,260 / 0.09,160 / 0.1,1)__static force (1N)__: Force is constant with 1N (like the start/end force of the dynamic force)

The problem is I can't get a non-linear solver to work.

**SOL106** doesn't work because I can't apply my surface-to-surface contact there. I did test this one with contact replaced with gluing. But then it still doesn't seems to use my dynamic force. The results for __dynamic force__ is the same as __static force (1N)__.

**SOL701** doesn't work because I can't apply my surface-to-surface gluing there.

**SOL601** fails:

SOL601 Advanced Non-Linear Static

[quote] T O T A L S O L U T I O N T I M E (SEC) . . . . . 218.65

MEMORY USED BY THE SPARSE SOLVER= 0.0mw ( 0.0mb)

TOTAL MEMORY USED BY THE PROGRAM= 34.4mw ( 275.2mb)

Checked in NX Nastran license feature nx_nas_advnlin_dsk.

*** END SOL 601 ***

*** FATAL ERROR: SOL 601 DID NOT FINISH SUCCESSFULLY.

*** ADVANCED NONLINEAR EXIT CODE 0 ***

*** ISHELL PROGRAM 'NXNA' COMPLETED ***

^^^ USER FATAL MESSAGE

^^^ ERROR IN ADVANCED NONLINEAR MODULE 0

^^^SOL601 FAILED [/quote]

SOL601 Advanced Non-Linear Transient

[quote] T O T A L S O L U T I O N T I M E (SEC) . . . . . 230.72

MEMORY USED BY THE SPARSE SOLVER= 0.0mw ( 0.0mb)

TOTAL MEMORY USED BY THE PROGRAM= 44.9mw ( 358.8mb)

Checked in NX Nastran license feature nx_nas_advnlin_dsk.

*** END SOL 601 ***

*** FATAL ERROR: SOL 601 DID NOT FINISH SUCCESSFULLY.

*** ADVANCED NONLINEAR EXIT CODE 0 ***

*** ISHELL PROGRAM 'NXNA' COMPLETED ***

^^^ USER FATAL MESSAGE

^^^ ERROR IN ADVANCED NONLINEAR MODULE 0

^^^SOL601 FAILED [/quote]

I use 3D mesh for every solver, I don't know if that can be the problem for eample the SOL601 solver? I don't know how to use 2D mesh becuse I get an error my mesh is faulty.

Labels:

11 REPLIES

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

10-04-2015 12:56 PM

Dear MarkosMark,

I see here many problems to solve: first at all if you plan to run any dynamic analysis (implicit Nonlinear or by modal superposition using modal frequency response) the model mesh would be clearly simplified at most possible, using 3-D tetrahedral mesh is not the way, the cost will be enormous in bot solution time & hard disc space, and the RAM memory requirements are high. I suggest to start with simply models, for instance 1-D beam elements for the frames and 2-D Shell elements for the plates, this way you can ignore local contact in the first phase, because your model is global. You need to arrive to a linear static solution to get a general idea of the mechanical behaviour of your structure, not trying to start your house by the roof!!, OK?. Also, 3-D solids can be meshed with Hexaedral elements instead tetrahedral, this way the model size will be x8-x10 times smaller.

In any case, if I solve you linear static analysis using load FY=420N (I have reversed source & target regions in your contact "no penetration" connector) I get a resultant displacement about 250mm, when the diameter of the beam tube is 16 mm. Well, this means that linear static results are useless because displacements are not small, for the level of load applied your structure requires a nonlinear analysis to consider large displacement effect.

Then you must solve your problem as minimum as nonlinear. Please note:

- If you load is static, then you can use advanced nonlinear static (SOL601,101).
- If you load is transient dynamic, then you must run nonlinear transient (SOL601,129).

In the first case the time is a dummy time, this is a static problem, remember, you can use a ramp function form (0,0) to (1,1). In the second case you must define a time curve as the one plotted. Here the time is real time.

In the **advanced nonlinear transient** you need to define the static & dynamic friction coefficients, the load associated to the time curve, the constraints, the time stepping, the solution strategy parameters (I suggest to use ATS), the output request, and ... patient!!, the solution time for dynamic analysis takes a lot!!. This is the reason why you need to mesh your problem in a smart way, not simply hitting mesh with TETs and you are done!!.

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
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-06-2015 10:01 AM - edited 10-06-2015 10:02 AM

I’ve simplified my problem, maybe this will help finding the way to get the results I’m looking for.

1. Fixed constraints

2. Fixed constraints

3. Surface-to-surface contact

4. Force load

These are two non-united beams. They are fixed at the face in 1 and 2. I’ve made a surface-to-surface contact at point 3 manually with two regions. And at point 4 I’ve applied a time depended force like applied before.

This force is created by defining the force in steps between 0 and 0.1 sec:

Time (sec) | Force (N)

0.00 | 1

0.01 | 200

0.02 | 350

0.03 | 400

0.04 | 420

0.05 | 400

0.06 | 260

0.07 | 320

0.08 | 260

0.09 | 160

0.10 | 1

I would like to see what the maximum values in my model will be. This can either be by just showing the maximum values over the given period/solution. Or just seeing the results step by step (at t=0, t=0.01, …, t=0.05, …, t=0.1)

Does this makes clear what I'm looking for? What solution type should I use for this?

(People around me are saying just to use a static force, but the results won't be the same. The displacement/stress will be totally different if I just apply this force for a short period, or I apply this force continuously)

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

10-06-2015 10:41 AM

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

10-08-2015 12:30 AM

So you are saying there is a difference between short period load and a continuous load. So what is the difference?

That would be inertia effect.

Therefore, Sol601129 is used for short period loading, because it accounts for the inertia effect. and Sol101 is used for continuous loading, by assuming the load is staticand no inertia.

Tuw

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

10-14-2015 11:33 AM

Thank you JimB! That looks like what I'm looking for. Both simulations (106 and 129) seem to deliver the same results at the same time (but 106 has much more increments)

But what is the difference between the two in results and setup?

When should I use 106 and when 129? Tuw mentioned above, 129 accounts for inertia effect, does 106 do this too?

And what did you change with both solutions from the standard setup?

I saw you added two Time Step Intervals: Static and Dynamic. And these steps are the same for SOL601-129 and SOL601-106

Did you add or change more? And how are these Static and dynamic steps used? Do I need to referrer to this Dynamic/Static somewhere?

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

10-20-2015 10:15 AM

@JimB I tried to reconstruct your file but I don't get results. Everything seems te be the same except this under S*olution > Case Control*:

- mine says __Time Step Intervals (0)__ while yours says __Time Step Intervals (1)__

What am I doing wrong?

See attachment

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

10-20-2015 01:48 PM

Edit the Solution. Under Case Control, to the right of Time Step Intervals (0), pick the *Create Time Step Intervals...* icon:

This will bring up the Time Step modeling object manager. You can create time steps in the top section of the dialog. Existing time step objects are shown in the middle section (Selection). Objects that are selected into the current solution are shown in the bottom (List).

In your case, two time steps are already created, but none are selected into the solution. You simply need to select one or more in the Selection area and pick the Add button in the List area to add them to the solution:

Note that the first item in the list area becomes the TSTEP card in the Nastran input deck. If additional items are selected into the list, they become continuation lines on the TSTEP card.

When you close this dialog, the edit solution dialog will now show how many items are selected into the list:

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

10-21-2015 09:05 AM - edited 10-21-2015 09:10 AM

@JimB ~~Okay thank you, that was the thing I missed. For SOL601-106 it works, but when I try this for SOL601-129 (static or dynamic) I don't get results. One thing that's mentioned in the log is:~~

~~WARNING Some output requests defined for solution "SOL601-129" are specified with sorting option "Default" or "SORT2". SORT2 results are not supported by Post Processing. These results may not be viewable.~~

edit: okay I found the problem. It should be __SORT1__ instead __default__ or __SORT2__. But looking through the output parameters I see some more differences:

*Contact result: Seperation Distance*

- standard is __None__, but you have __SEPDIS__

Is there some overview with settings that needs to be changed within different solutions?

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

10-21-2015 09:16 AM

SORT1/SORT2 and SEPDIS are output requests, not "settings". There is no "need" to "change" them as they have no bearing on the convergence of the solution itself, only what results the solver stores in the results file. The choice of output quantities is entirely up the the analyst based on what they are trying to get out og the analysis and what quantities they need to post process to do so.

Static analysis types default to SORT1 output. Transient analysis types default to SORT2. This is because historically, results were only captured at critical points on the model and were typically analyzed via time history XY plots.

The SEPDIS describer on BCTRESULTS asks the solver to store separation distance in addition to contact force and pressure. The decision to request it is up to the analyst. If you do not need it to post-process, then don't activate the option.

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc