Hello again ,
What i meant earlier is that the file run without any errors, because it sounded like you had problem getting it to run.
I run it today and yes it seem to stop after a certain frame. it is because the time step was small and the rigid part does not reach the golf ball, and time increment is very small ( i don't want to confuse you too much, i'm terrible at explaining things). Imagine the velocity of a ball is given to be 1 m/s, and the time you gave that ball to reach a target which is 1 metre away is only 0.5 seconds, the ball will never reach the target, you with me?
First of all i had to make few changes stated below:
(1)under the interaction defined between the surfaces I changed the Mechanical constraint to Penalty contact method.
(2)The element type of the rigid part and others were on "standard", which should be "explicit" because you are running an impact simulation and using a dynamic,explicit time step/
(3) For the Tie constraint , i changed the parameter under the Position Tolerance to "use computed default"
(4)The Predefined field velocity i removed it, because we already defined velocity under BC.
(5)I removed the Amp (under amplitudes) and used Instantaneous for the Amplitude
(6) Also, i have introduced a new boundary condition for the (moving) rigid part to be fixed (encastre) at the start of the second step.
(7) finally i changed the step time of the first to 0.013s, i did this because i know that the velocity is 15m/s, and to get the rigid part to move position of 0.2m in the (positive)x direction i will need a time step of 0.013 (0.2/15). I assumed that the rigid part will hit the gold ball until about the centre line( of the ball) and stop. You will need to change this to match what you are want to simulate. I also , changed the second step time to 0.04 seconds, to capture the ball moving due to the KE it gained from the impact. If i leave it as 1 second and the field output you requested is 20 equal intervals, then the result shown will be for each 0.05 seconds (1/20) which will display the ball after it hit the second rigid body and rebounced. Increase the number of the requested frames or decrease the step time for the secodn step to capture more frames for after the ball is hit.
I rerunt the simualtion and it was working until the impact happened, and then an error occured. It stated "The ratio of deformation speed to wave speed exceeds 1.0000 in at least one element"
I further investigated the cause and it seems the Rubber (caoutchou) material definition causes that error. I don't know why but i am guessing the definitions is wrong. Doubles check the data .
SO i decided to use the Resin material definition for the part (manteau)that is suppose to have the rubber and see if it worked.....and it did work just fine.
I am using 6.13-4 which is one the latest version of Abaqus i think. it will not open in your abaqus i don't think, as the backward capability is not supported. So i will attach the Input file instead , open it using File, import, model, then make sure that the file filter detects ".INP" files and open it.
I hope this helps. and no problem, I once was a student doing my MEng Dissertation and was modelling impact on laminated composites. I managed to do it thanks the to helpful FEA gurus here, so i would like to help others as much as i can to repay the debt.
