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
- Question about SOL 129 (time increments and displa...

Options

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

Highlighted
#

Question about SOL 129 (time increments and displacements graph)

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

07-13-2018 04:23 AM

Hello! I am a newbie in NX, so I ask for your help.

I don`t undesratand, what do *Number of Time Steps* and *Time Increment* exactly mean (they are set in Nonlinear Transient Parameters) in *NX Nastran - Structural Analysis Type - SOL 129 Nonlinear Transient Response*.

I tried to make a solution with a beam (you may find a folder with files in attachment). There was one Force = 10N, a fixed constraint, Number of Time Steps = 100 steps and Time Increment = 0.05sec. I don`t understand how to interpret a Displacements Graph (a pic below). While time is going, displacements must be growing up, but they are not. Also I don`t understand why the Graph is periodic after all I made a static Force (10N) only.

Don`t Steps like Cycles of applied force?

Another thing which is not clear for me is why in Results I got 3199 Increments (you may see it in .sim file in attachment).

Thanks in advance!

Regards

- Tags:
- Sol 129

4 REPLIES

Re: Question about SOL 129 (time increments and displacements graph)

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

07-13-2018 11:49 AM

SOL 129 is a dynamic transient solution. That means that delta time and damping come into play (compared to a static solution).

To answer your first question, the *Number of Time Steps* tells the solution how many steps to take and the *Time Increment* tells it how big each steps is. You model has Number of Steps set to 100 and Time Increment set to 0.05. So the total duration of the solution is 100 * 0.05 = 5.0 seconds. Note that this is the max value of the abscissa in the plot shown.

In your model, the full load is applied immediately at the first time step. In a dynamic analysis, this is essentially an impulse load that causes the structure to overshoot the "static" displacement. It then oscillates about the static displacement value. Without damping it takes a long time for this response to die out.

If you run a static solution (SOL 101) with the same boundary conditions, the peak Y displacement is 6.812mm:

If you look at your SOL 129 results, the peak is 13.492mm. You can eyeball the response plot and see that it is oscillating about 6.8. If run long enough for the ringing to die out, it will eventually reach 6.812.

If you slowly ramp the load throughout the duration of the solution, there is no overshoot and no ringing:

If you add damping to the solution, the oscillations die out quicker. This is 1% structural damping:

The updated .zip file has the SOL 101 run as well as two additonal SOL 129 runs - one with the load ramped over the duration and one with damping.

Re: Question about SOL 129 (time increments and displacements graph)

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

07-16-2018 09:43 AM

Thank you for your answer!

I didn`t notice that in SOL 129 average dispalcement is 6.8 mm, thank you.

But there are still some things not clear for me.

The first. If SOL 129 simulates the force only on the first step (acts on the beam once for 5 sec), why doesn`t average

displacement go to 0 or nearby in the end? Am I wrong if I say that when the beam get under the load, then the load is gone, the beam start ringing, but in the end it stops in the same position which it had in the beginning (or become a bit deformed if it is not enough elastic)? So 6.8 mm is a very big displacement for the beam not under load. I did not specify gravity.

The second. 10 steps and 100 steps give different dispalcements on the 5th sec (1.85 mm when 10 steps and near 6 mm when 100 steps). Mustn`t they be equal? (pics below) Conditions are all the same.

Unfortunately I can`t open your files, because my NX 11 tells me "Part file is from a newer version of NX".

.prt can be opened, but .fem and .sim can't.

Re: Question about SOL 129 (time increments and displacements graph)

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

07-16-2018 11:16 AM

In this model, the load is not acting in only the first step. Your force is applied as a static (non-time varying) load. This means that the load is present at all time points. In the original model, the full magnitude was applied instantaneously, so the displacement overshoots the static value. After the dynamic effects have died out, the load is still present so the displacement is the same as the static value (or the value where the load is slowly ramped to its full magnitude).

Simcenter 11 files are attached (Beam3.zip)

Re: Question about SOL 129 (time increments and displacements graph)

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

07-17-2018 01:45 AM

Thank you for answer!

Now your files are opening.

Follow Siemens PLM Software

© 2019 Siemens Product Lifecycle Management Software Inc