No results in explicit quais-static

[Anonymous]

Hello dear community,

So I was calculating some assemblies for my study, frequently with the explicit quasi-static solver, because of critic contacs and non-linear materials.

But recently I can't get any results from the solver. I don't know if the new Update 2021.2 is the reason but I think have this issue since the update.

I setup every case like before with timesteps in range of 0:0,01:0,1 (10 timesteps with no skips) and it's computing quite long, but the only result I get is for the timestep 0.00...0E+00 and thats not what I expect every time.

The first case here ist with some elastic materials:

I found a similar post ( /t5/inventor-nastran-forum/quot-explicit-dynamic-quot-no-time-steps-found-in-the-results/td-p/9774154 ) but it didn't helped. I tried a simulation with only steel material, but it's the same result (= no result):

I tried all cases with Implicit and Linear Static and I get converged results. But as far as I know the explicit should run as well.

Could it be that the new Update changed Parameters? I reset them before the calculations but it didn't helped.

The output files are attached, and so far as I observe it writes only one timestep but calculates a lot.

Thanks in advance.

Best,

Mert

[Anonymous]

I have something to add:

I decided to make some research by myself and I got a little workaround:

I build up an easy beam geometry and compared some solver options.

It seems that the option "Force" at the explicit quasi-static solver output causes this problem.

Here the results with the options strain and stress (same results with only stress):

I get clean results with all 10 timesteps.

And here the results for the option with force and stress (same results with only force):

Again no results and no timesteps solved. I attached both .out data for more informations.

It seems that the output options "Force" has an issue (at least for my AMD processor).

Is that a common problem or is this the normal solver reaction?

I learned that the explicit solver uses the kinetic-energy for solving reactional force, maybe it's a bug?

Best regards,

Mert

[John_Holtz · Accepted solution]

Hi Mert. Thanks for tracking down the source of the problem. I have reproduced it here, and I agree that explicit quasi-static with Force output activated is causing a crash. I will report the problem to the developers.

Note that you do not need to output the Force results unless the model includes beams or shells. Those are the only elements that have a force output.

(Correction: Shell elements do not create any force output either. The only reason to include the Force output is if the model includes beam elements.)

[tony_berset]

@John_Holtz 

Same problem here, with or without "Force" output. The issue appears after few analysis (for the same model), so initially it works, then it does not complete the "Writing results" process anymore :

I randomly encounter this problem on the 2025.0 Inventor Nastran release. I have Intel processors (no AMD). Is Autodesk still investigating on this problem ?

[John_Holtz]

Hi @tony_berset 

Please see the solution in this post: Solved: Enforced Rotation in Explicit Quasi-Static - Autodesk Community - Inventor Nastran. (See my message from 03-28-2024 plus or minus 1 day depending on your time zone and how the forum shows the dates 🙂.) The best that I know is the rigid connector (or maybe enforced motion) is causing a problem in quasi-static. The solution is to use the last duration calculated by the quasi-static analysis and run the analysis as an explicit dynamics.

John

[tony_berset]

Hi @John_Holtz ,

Thank you for this workaround, unfortunately the analysis in Explicit Dynamic takes approx. 13 hours instead of 15 minutes for Quasi-Static. As I understand, you have reported this quite recent issue to the developers team. May I ask you to keep me up to date as soon as a fix is released please ? I have many customers experiencing the problem.

An additional information for the developers: Most of the time, "Writing output results" process stop after only one "Writing" but randomly after few ones, but anyway it does not go to the end of the process.

[John_Holtz]

Hi @tony_berset 

I do not understand. Are you saying that Quasi-static runs to completion and gives results in 15 minutes?

Quasi-static runs the same solver as Explicit Dynamics. The difference is Quasi-static runs the analysis multiple times and increases the duration each time; Explicit Dynamics runs the analysis once using the duration entered. The quasi-static analysis must take longer to run than the Explicit Dynamics. My description of how to simulate a quasi-static analysis using the explicit dynamics may have been lacking details. Sorry. The output file for the quasi-static analysis will include lines like this:

   Trial Number 1, Solving for Trial Duration = 2.893e-05
   1st Trial Duration  = 2.893E-05 set to 1000 times the intial Courant Stability Limit of 2.893E-08


           Time     Static   Free Kinetic Internal   Viscous  External    Elapsed    Remaining
    Inc    Step      Time       Energy     Energy    Energy     Work     Wall Time   Wall Time
      0  2.89e-08  0.00e+00    2.64e-09   0.00e+00  0.00e+00  0.00e+00  0 00:00:00         n/a
     50  2.89e-08  5.00e-02    2.18e-04   1.95e-04  8.06e-09  4.12e-04  0 00:00:00  0 00:00:06
...
   1000  2.89e-08  1.00e+00    1.36e-04   1.34e+00  8.86e-09  1.34e+00  0 00:00:08  0 00:00:00
  >>>>>> Writing Selected Results Issue: ExplDyn3:1.00055E+00 <<<<<<
   1001  2.89e-08  1.00e+00    1.29e-04   1.34e+00  8.75e-09  1.34e+00  0 00:00:08  0 00:00:00

   Trial     Mean Free          Mean        Maximum       Last          Mean      Actual    Restricted
  Number  Kinetic Energy  Internal Energy    Value     Convergence  Convergence  Multiplier  Multiplier
     1       6.304e-03       4.984e-01     1.265e-02     9.839e-05   1.265e-02   1.836e+00   1.836e+00
  >>>>>> Writing Selected Results Issue: ExplDyn3:0.00000E+00 <<<<<<

   Trial Number 2, Solving for Trial Duration = 5.312e-05


           Time     Static   Free Kinetic Internal   Viscous  External    Elapsed    Remaining
    Inc    Step      Time       Energy     Energy    Energy     Work     Wall Time   Wall Time
      0  2.89e-08  0.00e+00    2.32e-10   0.00e+00  0.00e+00  0.00e+00  0 00:00:00         n/a
     50  2.89e-08  2.72e-02    1.99e-05   1.77e-05  7.56e-10  3.76e-05  0 00:00:00  0 00:00:11

The lines beginning with "Trial Number N, Solving for Trial Duration = t" give the time that you want to use for the explicit dynamics duration. In this example, line 19 is for the second trial. The duration is 5.312E-5, so I would round that off to 5.5E-5 for the explicit dynamics analysis. 

The column "Static Time" is not the duration of the analysis. Normally the second column is in fact the current time, but for the quasi-static analysis this column is normalized so that the real duration (5.312E-5) looks like it has a total duration of 1.0E+0 seconds.

An explicit analysis with a duration of 5.5E-5 will run faster than a quasi-static analysis that runs one analysis for a duration of 2.89E-5 (line 1) and a second analysis for a duration of 5.31E-5 (line 19).

Hope this clarifies the quasi-static analysis.

John

[tony_berset]

Hi @John_Holtz ,

Yes, at the first run the Quasi-static analysis takes only 15 minutes to complete (then it does not complete anymore due to the problem mentionned previously in this post).

Basically, I change the analysis type from Explicit Quasi-Static to Explicit Dynamic and I set a total duration time of 1 second. When I run it the "Remaining Wall Time"  is far longer than 15 minutes (approx. 13 hours). So either I missed something in the Dynamic settings or an Explicit Dynamic simulation is just more complex to calculate than a Explicit Quasi-static (what it would make sense to me).

Thank you for the clarifications.

Tony

[John_Holtz]

Hi @tony_berset 

The duration of the analysis is not 1 second, even though the output does imply that the duration is 1 second. The real duration is probably on the order of 0.0005 seconds which is why it is able to run in 15 minutes. (If the second trial would run, it would take longer than 15 minutes. Then the third trial would take even longer, and so on.)

The first column in the output file is the increment ("Inc") or step. It generally increases in steps of 50. How many steps were used for the first trial? 

The second column is the time step size ("Time Step"). It is generally on the order of 1E-8. Multiply the number of steps at the end of trial 1 and the time step size, and that will give you the duration. (Or if these lines are still output, you can look at them which shows the total duration. 🙂)

Trial Number 1, Solving for Trial Duration = 2.893e-05
1st Trial Duration  = 2.893E-05 set to 1000 times the intial Courant Stability Limit of 2.893E-08

Choose the longest duration that gives a reasonable runtime. Change the load curve to apply the loads gently. (I use a half-sine wave to start slow, speed up in the middle, and end slow. Kind of like Figure 4 on the page Section 29: Explicit Quasi-Static Analysis.)

John