I need help 1

[Dothraki]

thread799-180576

Hi everyone,

I'm having troubles runniing a simulation of a golf ball hitting a rigid plan

I get this warning message

"FOR AN Abaqus/Explicit ANALYSIS CONTAINING A *HYPERELASTIC OR *HYPERFOAM MATERIAL WITH *VISCOELASTIC PROPERTIES, THE STRAIN ENERGY OUTPUT INCLUDES THE CONTRIBUTION OF VISCOUS DISSIPATION. SPECIAL CARE SHOULD BE EXERCISED WHEN INTERPRETING STRAIN ENERGY RESULTS.

There are 2 warning messages in the data (.dat) file. Please check the data file for possible errors in the input file."

I have also attached my cae file please help.

 

[Mohcine]

Hi,


Is the simulation not running at all? do you only get warnings but no error messages.
Sometimes, you can ignore the warning messages but just be aware of them.

I have just managed to get it the model you sent to run just fine.

I got to say, i am not a expert in this field, but i have been working as an FEA engineer in my current role for about 10 months, so i might be able to help.

Regards Mo

 

[Dothraki]

Hi Mohcine,

Thank you for Your message, You are a life saver my friend.
When I submit the job, I do not get errors just warning messages, but the job takes forever, it keeps running. I left it overnight the other day and in the following morning it was still running.

Would it be possible for you to attach the file you successfuly managed to run and send it back to me.
Again thank you Mohcine for your time and your help.

Regards S

 

[Mohcine]

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.

 

[Dothraki]

Hello Mohcine,

I can't thank you enough for your precious help, I understood every step you outlined in your recent post and I realised all the mistakes i have made so far.

for the material definition I will invistigate the properties and parameters. and will let you know of the results.

For the Inp.file you sent me I followed exactly your instructions, but when I started the job I got this error message

"Value for parameter elset cannot be more than 80 characters"

Analysis Input File Processor exited with an error.

So I investigated the problem in the data file here's a snapshot:

*material, name=MATERIAL-RÉSINE
*density
*elastic
*material, name="Material-Alliage aluminium"
*density
*elastic
*mass, elset="ASSEMBLY_Part-Club de golf-1__PickedSet6_Set-1_Inertia-masse club__"

***ERROR: VALUE FOR PARAMETER ELSET CANNOT BE MORE THAN 80 CHARACTERS
LINE IMAGE: *mass, elset="ASSEMBLY_Part-Surface rigide
plane-1__PickedSet6_Set-3_Inertia-masse plan rigide__"
*mass, elset="ASSEMBLY_Part-Surface rigide plane-1__PickedSet6_Set-3_Inertia-masse plan rigide__"
*surfaceinteraction, name=INTPROP-FROTTEMENTS
*friction
*solidsection, elset=ASSEMBLY_PART-NOYAU-1_SET-1, controls=EC-1, material="Material-Alliage aluminium"
*solidsection, elset=ASSEMBLY_PART-MANTEAU-1_SET-1, controls=EC-1, material=MATERIAL-RÉSINE
*solidsection, elset=ASSEMBLY_PART-PEAU-1_SET-1, controls=EC-1, material=MATERIAL-RÉSINE
*sectioncontrols, name=EC-1, hourglass=ENHANCED

I'm not sure what to do at this point, also I managed to get the latest version of abaqus 6.13 installed on my pc. so I was wondering if you could send the working cae file.

I'm so sorry if I have taken so much of your time.

Best Regards SS

 

[Mohcine]

I have attached the CAE, hopefully it will run without a problem.