I cannot run my model
Hello,
I'm trying to perform a simulation of a rigid wall which is coming towards a structure and hits it and deforms it to get the kinetig energy. The problem is that I get below Error in Model checker:
And I get below Errors after starting the run.
Could someone help me to solve these issues and get the model running?
Enclosed you can find my simulation file.
Thank you in advance!
Best Regards,
Sajad Ahmadimajd
Answers
-
You haven't left a gap between your impactor and the component, TYPE7 needs a physical space between main and secondary, if you back the impactor off 1mm it is running.
However:
There are a number of other issues with the model
The contact should have gapmin set higher, 0.001 is too small, I would suggest 0.1mm as a minimum
Runtime is set as 15s (very long for explicit, and doesn't seem to correspond to duration for IMPDISP)
Some of your elements are very small, giving timestep of around 1.5e-8 (very small)
worst is this one 144434, but mesh has many such small elements
so it would take many hours to run (over 6 months on my laptop!)
Also, your material parameters look odd, strain at UTS is set as 19600% should be <100% at most
Good luck
I attached my revised version with impactor backed off, some interface changes (gapmin increased) and strain at UTS set at 0.2 (20%) it starts, and begins to run, but I did not correct any mesh issues or runtime or displacement values as I don't know your intent?
1 -
Paul Sharp_21301 said:
You haven't left a gap between your impactor and the component, TYPE7 needs a physical space between main and secondary, if you back the impactor off 1mm it is running.
However:
There are a number of other issues with the model
The contact should have gapmin set higher, 0.001 is too small, I would suggest 0.1mm as a minimum
Runtime is set as 15s (very long for explicit, and doesn't seem to correspond to duration for IMPDISP)
Some of your elements are very small, giving timestep of around 1.5e-8 (very small)
worst is this one 144434, but mesh has many such small elements
so it would take many hours to run (over 6 months on my laptop!)
Also, your material parameters look odd, strain at UTS is set as 19600% should be <100% at most
Good luck
I attached my revised version with impactor backed off, some interface changes (gapmin increased) and strain at UTS set at 0.2 (20%) it starts, and begins to run, but I did not correct any mesh issues or runtime or displacement values as I don't know your intent?
Hello Paul,
thank you for your inputs and corrections. I changed the movement type to initial velocity (15 m/s) and changed the run time to 0.05. The problem that I am facing now is that the run time is very long, and I have no idea why. Could you maybe help me with that?
I attach my input files.
Many thanks in advance!Best regards,
Sajad
0 -
Sajad Ahmadimajd said:
Hello Paul,
thank you for your inputs and corrections. I changed the movement type to initial velocity (15 m/s) and changed the run time to 0.05. The problem that I am facing now is that the run time is very long, and I have no idea why. Could you maybe help me with that?
I attach my input files.
Many thanks in advance!Best regards,
Sajad
The stable timestep in your model is quite small (around 1.5e-8s) this is due to element size, the stable timestep is calculated based on smallest element size/speed of sound in material (e.g. element size of 5mm gives approx 1e-6s timestep for steel) speed of sound is sqrt (E/Rho). In your model you have elements with size around 0.2-0.3mm, so timestep is small.
You can speed up the model in a few different ways:
Use mass scaling: By setting /DT/NODA/CST in engine, you can 'cheat' the timestep calculation by adding mass (increasing effective density in the calculation)
Use multiple threads, run the model on more CPU (use e.g. -nt 4 on submission line)
Modify the mesh to increase element size
In the attached, I modified your model a little: I swapped the main/secondary on your contact (wall should be main here), I changed the model units to match your input (makes no functional difference, just neater!), I put the initial velocity on all nodes of the wall. And I added a nodal timestep control to increase timestep to 1.2e-7s adding 4-5% mass (so your job should run approx 9x quicker).
For mass scaling, because your beam is static, you could increase timestep even more at expense of more added mass is you wanted to.
Another couple of observations: The way you have this set up right now, the wall has very little mass/kinetic energy really, so it will just bounce off, also you have no failure model set up for the beam (material values won't erode solid elements) if you want to see elements failing, you should add e.g. a /FAIL/BIQUAD for the beam material
0 -
Paul Sharp_21301 said:
The stable timestep in your model is quite small (around 1.5e-8s) this is due to element size, the stable timestep is calculated based on smallest element size/speed of sound in material (e.g. element size of 5mm gives approx 1e-6s timestep for steel) speed of sound is sqrt (E/Rho). In your model you have elements with size around 0.2-0.3mm, so timestep is small.
You can speed up the model in a few different ways:
Use mass scaling: By setting /DT/NODA/CST in engine, you can 'cheat' the timestep calculation by adding mass (increasing effective density in the calculation)
Use multiple threads, run the model on more CPU (use e.g. -nt 4 on submission line)
Modify the mesh to increase element size
In the attached, I modified your model a little: I swapped the main/secondary on your contact (wall should be main here), I changed the model units to match your input (makes no functional difference, just neater!), I put the initial velocity on all nodes of the wall. And I added a nodal timestep control to increase timestep to 1.2e-7s adding 4-5% mass (so your job should run approx 9x quicker).
For mass scaling, because your beam is static, you could increase timestep even more at expense of more added mass is you wanted to.
Another couple of observations: The way you have this set up right now, the wall has very little mass/kinetic energy really, so it will just bounce off, also you have no failure model set up for the beam (material values won't erode solid elements) if you want to see elements failing, you should add e.g. a /FAIL/BIQUAD for the beam material
Here, added mass of 1 tonne to barrier, added some arbitrary failure to solids and moved barrier closer to beam to save the dead time.
0 -
Paul Sharp_21301 said:
Here, added mass of 1 tonne to barrier, added some arbitrary failure to solids and moved barrier closer to beam to save the dead time.
Hello Paul,
I wanted to try another model with the same setup, but unfortunately I cannot get it to run.
The idea is that the wall moves 160 mm towards the structure and the reaction force is the favorable parameter at the end. I have another problem as well with the material. I chose an elasto plastic with Plas John for aluminum, but it is so brittle and the wall just smashes the elements and they fly away. I expect to see deformation, but I don't know why it doesn't deform and instead breaks.
In attachment, you can find my radioss files
I'm really looking forward to your response and help.Thank you in advance!
Best regards,
Sajad
0 -
Sajad Ahmadimajd said:
Hello Paul,
I wanted to try another model with the same setup, but unfortunately I cannot get it to run.
The idea is that the wall moves 160 mm towards the structure and the reaction force is the favorable parameter at the end. I have another problem as well with the material. I chose an elasto plastic with Plas John for aluminum, but it is so brittle and the wall just smashes the elements and they fly away. I expect to see deformation, but I don't know why it doesn't deform and instead breaks.
In attachment, you can find my radioss files
I'm really looking forward to your response and help.Thank you in advance!
Best regards,
Sajad
In attached, I made the following modifications:
Removed the 2 or 3 completely flat tetra that were being deleted due to negative volume
Added a self contact (TYPE25) to the beam
Set Idel=2 on both the new contact and the existing TYPE7 (so eroded elements are also removed from contact)
Set the /IMPDISP on the main node of the RBODY (should not be set on secondaries)
The beam bends on impact rather than purely crushing, because the cross section is not symmetrical (there is a loadpath only really on one side) it induces bending in compression
0 -
Paul Sharp_21301 said:
In attached, I made the following modifications:
Removed the 2 or 3 completely flat tetra that were being deleted due to negative volume
Added a self contact (TYPE25) to the beam
Set Idel=2 on both the new contact and the existing TYPE7 (so eroded elements are also removed from contact)
Set the /IMPDISP on the main node of the RBODY (should not be set on secondaries)
The beam bends on impact rather than purely crushing, because the cross section is not symmetrical (there is a loadpath only really on one side) it induces bending in compression
Now, in addition, added friction to wall and modified constrained end to be rigid to help with force extraction (TH request is there for it)
With Friction, the beam is eroded again, but the plastic strain to fail in compression (1.0 with the biquad settings, i.e. c1 = c3 * 5 with mflag set = 4) is being met
The failure parameters were just made up by me for the earlier model, if you have better data then you may substitute it
0
Altair Employee