Issue with time scaling

[nickkuuttila]

Hello,

I am currently having an issue with a relatively simple simulation. I am attempting to deform a small solder sphere between two rigid plates in Abaqus explicit. I fixed one plate and applied a velocity boundary condition to the other

I started off having an issue where the simulation would not run. The STA file said that the simulation required a large number of time steps (about 2 million) to solve. I solved this problem by scaling the time of the simulation down and increasing the moving plates velocity. eventually I was able to obtain a usable ODB file after scaling the time of the simulation down. When I opened the ODB and attempted to view the deformed state of the model a message appeared saying "results for the current deformed variable are not available for one or more nodes contained in the model. deformations at such nodes are assumed to be zero".

After making sure the plates rested directly on the sphere in the initial assembly, I was able to get this message to go away but when I viewed the deformed state of the model the displacement of the plate was not even close to what I set it to via the time of the simulation and the velocity of the moving plate.

I have checked my INP file several times and I don't think there is any thing wrong so I'm kind of at a dead end on what to try next. I am quite new to time scaling and Abaqus as a whole so I would greatly appreciate anyone's input on how to resolve this issue.

Thanks,

Nick

 

[compositesFEAguru]

Hi Nick,

Try applying a finite displacement boundary condition with a ramped amplitude curve (default in Explicit is step) instead of a velocity. Using the same time step, see if everything looks correct, then move on to velocity. It may be easier to resolve contact, density, etc. potential errors by starting with a "simpler" simulation.

Regards

Firehole Composites

http://www.firehole.com

 

[nickkuuttila]

Thanks for the reply!

I tried changing the velocity BC to a disp BC. I re-ran the simulation and when I went to check displacement the same message came up
"results for the current deformed variable are not available for one or more nodes contained in the model. deformations at such nodes are assumed to be zero"

I also saw a warning in the DAT file that said
"***WARNING: THE OPTION *BOUNDARY,TYPE=DISPLACEMENT HAS BEEN USED; CHECK STATUS
FILE BETWEEN STEPS FOR WARNINGS ON ANY JUMPS PRESCRIBED ACROSS THE
STEPS IN DISPLACEMENT VALUES OF TRANSLATIONAL DOF. FOR ROTATIONAL
DOF MAKE SURE THAT THERE ARE NO SUCH JUMPS. ALL JUMPS IN
DISPLACEMENTS ACROSS STEPS ARE IGNORED"

I am confused by this because I have two steps so there can not possibly be displacement jumps between my steps other than my prescribed simulation.

Do you have any other thoughts about what might be wrong?

Thanks,

Nick

 

[compositesFEAguru]

You need to apply the displacement BC with an amplitude curve.

Firehole Composites

http://www.firehole.com

 

[nickkuuttila]

I did use this method for applying my boundary condition. I applied a ramp amplitude to a displacement BC.

The net effect should be a constant velocity displacement over the time period of the step.

I am still having the same issue however.

Thanks,

Nick

 

[compositesFEAguru]

Copy and paste your *Amplitude and *Dynamic keywords so I can look at how you are defining your amplitude.

Firehole Composites

http://www.firehole.com

 

[nickkuuttila]

*Amplitude, name=Amp-2
0., 0., 0.001, 1.

*Dynamic, Explicit, fixed time incrementation
, 0.001

Again, thanks for your help.

Nick

 

[compositesFEAguru]

That all seems correct. I'm not sure why you would be getting the message "results for the current deformed variable are not available for one or more nodes contained in the model. deformations at such nodes are assumed to be zero". Look for any additional errors/warnings in your .dat, .sta, .msg files. Don't worry about:

***WARNING: THE OPTION *BOUNDARY,TYPE=DISPLACEMENT HAS BEEN USED; CHECK STATUS
FILE BETWEEN STEPS FOR WARNINGS ON ANY JUMPS PRESCRIBED ACROSS THE
STEPS IN DISPLACEMENT VALUES OF TRANSLATIONAL DOF. FOR ROTATIONAL
DOF MAKE SURE THAT THERE ARE NO SUCH JUMPS. ALL JUMPS IN
DISPLACEMENTS ACROSS STEPS ARE IGNORED

My guess is that a node(s) is not constrained properly somewhere in your model. Try making changes to the BCs, possibly the sphere or rigid plates do not have enough constraints on them and there are rigid body motions. Overconstrain and work backwards.

Firehole Composites

http://www.firehole.com

 

[nickkuuttila]

Finally got it to work! I guess the sphere was rotating between the two plates I applied a roughness interaction property so that the sphere would not move as the plates were displaced and the simulation worked!

Thanks for the advise compositesFEAguru.

Nick