Learning Forum

[bobsik641]

Hi everyone!

 

I need some help with Explicit Dynamics.I need some help with Explicit Dynamics. I’m doing a projectile penetration/mushrooming simulation. When I try to solve it,it shows an error: TIME STEP TOO SMALL. I tried to manipulate with the solution setting and meshing (I’m not good at meshing though) but to no avail.

Here are some details:

Materials: plate explicit steel, projectile explicit brass, both eroding on max plastic strain

Geometry: projectile L=20mm, d=8mm, plate D=200mm, t=10mm, distance between the two 20mm, plane symmetry option used (90deg. is considered in computations)

 

Conditions: initial velocity 4e5 mm/s, plate outer edge fixed

 I don't really want the mesh to be coarse on the bullet, as I want to inspect its shape after the collision.

I set erosion on material failure (max strain defined in the engineering data).

To mesh the structure, I did the following:

generate general, sizing 2mm applied to the bullet, sizing 2mm with sphere of influence to the plate centre, sizing 4 elements along the plate thickness. Refining didn't help.

 

 

 

[Karthik Remella]

Hello,

Moving this question to the Structural Mechanics thread for more visibility on this question.

Thank you.

Best,

Karthik

[peteroznewman]

In the Geometry program, move the projectile tangent to the plate to start the simulation.

Make the elements about four times smaller.

Note: you cannot type the word   b u l l e t   on the site, it is a prohibited word.

[bobsik641]

It took a lot of time until I found out that word's prohibited. I will remodel the geometry.

 

 

Meanwhile, I performed a very similar simulation wherein there was some distance between the "projectile" and the plate. It was solved without any problems. 

Have you got any other tips on how to set the Explicit Dynamics solver settings (in general)?

[bobsik641]

I refined the mesh up to size=0.5mm. I see the quality is good only in the very vicinity of the impact zone.  Is that fine? I reached the max element No limit.

The end time is set to 1e-4s. All other time settings are programme controlled. The same error TIME STEP TOO SMALL appeared.

When I changed the mesh sizing to 0.7mm, the previous error got replaced by the following one

License acquired!
Checking model setup.....Please wait
Generating External Faces ...... please wait
Initializing.....Please wait
Finished model setup.....
Initializing slaves....
Cycle:        0, Time:  0.000E+00s, Time Inc.: 1.399E-08s, Progress:   0.00%, Est. Clock Time Remaining: -
Cycle:        1, Time:  1.539E-08s, Time Inc.: 1.539E-08s, Progress:   0.02%, Est. Clock Time Remaining: -
 
 
SIMULATION ELAPSED TIME SUMMARY
 
EXECUTION FROM CYCLE        0 TO        1
ELAPSED RUN TIME IN SOLVER =      3.79867E-01 Minutes
TOTAL ELAPSED RUN TIME     =      3.79900E-01 Minutes
JOB RAN OVER     4 SLAVES
JOB RAN USING Intel MPI
JOB RAN USING DECOMPOSITION AUTO
 
Problem terminated .... no cell controlling time step

 

Mesh with size=0.5mm below

 

[peteroznewman]

The benefit of eliminating the gap between the projectile and the plate is you don't spend a lot of time waiting for the solver to move the projectile up to the impact position. You can do that more quickly in CAD.

Under Output Controls, set the Result Number of Points to 500 instead of 20.

Here are the Google search results of the 19 time where the search term explicit "time step too small" was found. See if there are any useful suggestions in them.

[bobsik641]

None of the advices mentioned there solved the problem . I tried to change the MIN timestep from programme controlled to 1e-15s (or even 1e-25s), but it didn't helped much. Please find attached my project archive. I'd be very grateful if you could please adjust the settings. If you don't have time to solve that, that's fine, I'll do that.

What's important for me is to learn how to properly set such simulations , not just to solve that one. I know that a MIN time step is such a time interval in which an elastic wave travels at most 1 MIN cell length/diameter. The MIN characteristic length of my mesh is 4e-2 mm. So according to the CFL condtition dt=6e-9s.

Some people suggest to get rid of the smallest mesh elements... The meshing in the impact zone is fairly homogeneous, while the projectile meshing comprises mainly "triangular" elements of rather equal sizing. I've no idea how to get rid of that 4e-2mm element(s)...

 

I can see @SandeepMedikonda is experienced in the matter of Explicit Dynamics. That's how I tag people?

 

I very much appreciate your help.

[peteroznewman]

Use the Mesh Metrics to see the elements with the smallest characteristic length.
Click on the left most bar and the elements highlight.

Slice the plate to create better shaped elements.

You need better elements in the projectile also. You can easily double the characteristic length with a better mesh.

[peteroznewman]

I found that simply using the Body Fitted Cartesian Mesh control allows the model to run without error. It seems the error was due to poor element shapes.

  

[bobsik641]

I never would have thought about that. I removed all the smaller elements and reran the simulation, but the same ## warning error appeared. I will apply your method and I will let you know about the outcome. 

I appreciate your help.

EDIT: I applied your mesh settings. It generated some low-quality mesh on the outer surface of the "projectile", however I quickly managed to refine it using Inflation method.

I very much appreciate your help. Thank you, have a nice one

[Tenkist]

hi

i have same problem, how to create that kind of mesh? I made something similar in meshing tool with cutcell method, but i don't know how to import mesh to explicit.

[bobsik641]

The mesh is imported automatically when you're using Explicit Dynamics. Please read the thread for more info on how to mesh that geometry.

[Tenkist]

I don't mean to be rude, but if I knew where to read about it, I wouldn't ask. I don't know what mean "automatically" I can import mesh data to AUTODYN, but there is no option to import to explicit, anyway, cutcell is for fluent solver so i don't know if it would work, that why i would liek to know how you did it. I can't find cartesian method.