Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
I want to make a human head impact analysis in Mechanical Simulation 2012. I have nonlinear materials and so i use the "MES with nonlinear materials" as the type of analysis. I meshed the model and pressed check model. Everything is ok and there are no errors. I want to hit the head with a simple cylindirical element like shaft during 0,2 second and want to determine the stresses and the displacements. But i don'r know how to make it.
Will i draw a cylindirical shaft as a new part and give it a speed? Or without a new part will i put some nodal forces to the head surface and apply it for 0,2 seconds? Will it be true?
I want to take your suggestions. All of them is important for me.
Ok. Thanks for your advice. I hadn't realized that. It would be able to be a very big problem. I corrected it. I added "E-9" value to all material's density. Thank you so so much.
Is there a problem, in my opinion there is a problem in the analysis settings? I couldn't decide the time steps. When i choosed a constant time step i couldn't get the results. The program ends in a short time and gives no result. When i didn't choose constant time step it runs succesfully. Can you give some advice about time step please?
And the other problem is may i see the stress results in graph form? For example i want to see a part's displacement or stress graphic at the results. Is it possible?
Compared with the mass density of ASTM A36 steel: 7.85e-009, 1.133e-009 might be an appropriate value for the material you want to use.
I would recommend that a constant time step not be used for nonlinear problem, especially for nonlinear contact models.
I have finished the simulation of impact process and stopped the simulation of bounce-back process: a total duration time of 2s is too long for the large impact model, and 0.3s is enough.
Considering the large velocity, a capture rate of 100 is recommended.
I will update the contact setting changes once the simulation with a duration of 0.3s is done.
Hi. I saw an unexpected error a few minutes ago. Before the impact begins while the shaft was approching the head a stress is occuring on the front-bottom side (mandible) of the skull . The contact didn't occured but a stress occured. Why? Is there a bug?
Is the stress value large? If it is very small (for example, < 1.d-5, considering you might not use gravity) and just is larger than the other areas, then it might be fine.
I uploaded a file (tezizleme4_new.ach) to the same folder which you created. The file does not contain the results because of the size. You can rerun the model and check the contact pairs for contact setting changes.
Thank you very much Mr Shoubing, I run your new file and about 2 hours it's running and %45 of the simulation completed yet. According to your simulation with your computer's hardware Is this duration fast or slow? If my computer is slow what can i do for improving it? My hardware is i7 cpu with 3.0 GHz, 24 Gb DDR3 ram, 2 TB raid harddrive, 768 MB-384 Bit vga. While i was waiting new file from you i run some simulations and i observed an error again. After the impact the stresses on the head keep rising (increasing). I ran like 0.3 s, 1s, 2s, 3 s and 5 seconds of simulation times and in all simulations the stresses keep increasing by time. But in fact after the impact the stresses must be decreased. İn your opinion where i made a mistake? Thanks.
In the new file that I sent to you. I forgot to remove the gravity or to change the load curve. You can change this by yourself:
(1) If you don't need gravity, you can change "Acceleration due to body force" to 0.
(2) If you need gravity, you need change the load curve to
(0,1)->(0.3,1)
Shoubing
ramses061 wrote: Thank you very much Mr Shoubing, I run your new file and about 2 hours it's running and %45 of the simulation completed yet. According to your simulation with your computer's hardware Is this duration fast or slow? If my computer is slow what can i do for improving it? My hardware is i7 cpu with 3.0 GHz, 24 Gb DDR3 ram, 2 TB raid harddrive, 768 MB-384 Bit vga. While i was waiting new file from you i run some simulations and i observed an error again. After the impact the stresses on the head keep rising (increasing). I ran like 0.3 s, 1s, 2s, 3 s and 5 seconds of simulation times and in all simulations the stresses keep increasing by time. But in fact after the impact the stresses must be decreased. İn your opinion where i made a mistake? Thanks.
Change the duration to 0.28s, and then you can finish the simulation in 3-4 hours, where impact has happended already. You might notice that after 0.28s, the simulation is cut to 5th level of time step, while there is no contact and there is only large rotation of 3D kinematic part (part 44).
So you can reduce duration to 0.28s, and then either remove gravity or use the load curve 1: (0,1) ->(0.28,1).
If you are using previous load curve, (0,0)->(2,1), then after impact and there is no contact, while the gravity is still increasing.
Moreover, after impact, the deformation might continue becuase of the acceration and velocity (since we are using MES - dynamic implicit) and then results in some stress change, but this stress changes should be not so severe. However, the stress on the contact area should have maximum stress when impact.
I did simulate the case without velocity and the case with velocity of load cureve (0,1)->(2,1). Both of them has maximum stress when impact on the contact area.
. The contact didn't occured but a stress occured. Why? Is there a bug?
