Rotation in Abaqus/Explicit and It's Side Effects ... 1

[yassou]

Hi everybody
As far as i remember when i work with Abaqus Dynamic-Explicit or Dynamic-Explicit-Temperature Steps With One or Two or ... Part (Solid or Shell) Rotation, Below Problems will be appeared:
1) Computational Problem, Have To much Increments in simulation and if you look at the "Status File", you can see this Warning:

***WARNING: THE ANALYSIS NEEDS AN EXTREMELY LARGE NUMBER OF INCREMENTS (MORE
THAN 2,000,000). CHECK THE PROPERTIES OF THE MOST CRITICAL
ELEMENTS AND THE DATA FILE FOR WARNING MESSAGES.

2) Double Precision, To have more accuracy, You should activated the DOUBLE PRECISION from job module and this option make simulation have Computational Problem (Back to Number 1). If you didn't active it you see below Warning in "Status File":

***WARNING: THE ANALYSIS MAY NEED A LARGE NUMBER OF INCREMENTS (MORE THAN
300000), AND IT MAY BE AFFECTED BY ROUND-OFF ERRORS. RUNNING THE
DOUBLE PRECISION EXECUTABLE IS RECOMMENDED.

3) Elements with Rotational Degrees, are limited (Solid and Shell have not a Rotational Degrees), Then you need to use Tools Like "Rigid Body" or "Tie", And they have their own problems. Eventually using this kind of tools make simulation to have Computational Problem (Back to number 1).
4) Damage of that part (with rotation) make simulation incredibly Computational (Respect to the Type, Size and Number of Elements).
5) ....
Now, Is there any way to simulate Rotation in Abaqus/Explicit with new approach to have less Computational Time ?
With Best Regards.
yassou.

 

[akabarten]

Hi,

***WARNING: THE ANALYSIS NEEDS AN EXTREMELY LARGE NUMBER OF INCREMENTS (MORE
THAN 2,000,000). CHECK THE PROPERTIES OF THE MOST CRITICAL
ELEMENTS AND THE DATA FILE FOR WARNING MESSAGES.

This warning message is related to small time step in your analysis.
Time step depends on element size and material data not on active rotation.

DOUBLE PRECISION from job module and this option make simulation have Problem

How does double precision make computational problem?
It can only increase time of simulation.

Solid and Shell have not a Rotational Degrees

All shells have rotational degree of freedom.

Is there any way to simulate Rotation in Abaqus/Explicit with new approach to have less Computational Time

I do not think your problem is related to rotation.
To speed up simulation with Abaqus/Explicit you can:
- improve quality of your mesh to use elements as big as possible
- check all material data to use consistent system unit
- use mass scaling
- is possible use smaller step time (quasi-static simulation vs dynamic simulation)
- is possible use rigid bodies for parts you do not expect high deformation and your are not interesting in results

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[yassou]

Hi akabarten
Thanks for reply.

1- improve quality of your mesh to use elements as big as possible
2- check all material data to use consistent system unit
3- use mass scaling
4- is possible use smaller step time (quasi-static simulation vs dynamic simulation)
5- is possible use rigid bodies for parts you do not expect high deformation and your are not interesting in results

I should say my simulation is Dynamic-Explicit-Temperature with Element deletion and high speed Rotation of one part, and other part have contact with the part one.
Now:
Where can i found any information about number 3 (Mass Scaling), can i use it with that kind of configuration ?
Can you tell me more information about number 4 and 5, can i use it with that kind of configuration ? ?
With Best Regards.
yassou.

 

[akabarten]

Hi,

Where can i found any information about number 3 (Mass Scaling), can i use it with that kind of configuration ?

1. check Abaqus documentation: Abaqus Analysis User's Guide, 11.6.1 Mass scaling
2. check attached pdf file
For sure can be use it with dynamic-explicit analysis but I do not know how it influence temperature calculations.

Can you tell me more information about number 4

2. check attached pdf file
In principals in quasi-static analysis you use lower time of load.
For instance you apply force over 10ms instead 1000ms (1 second) to cut town calculation time.
If phenomena you are simulating is strongly time depended (temperature distribution over time?) I think you can not use it.

Regards,
Bartosz


VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Mustaine3]

Quasi-static analysis with A/Explicit are explained in the Getting Started documentation.