fake Stress in Hyperview
hi my Dear
I simulate impact (Intrusion test) with front Door and Pole impactor.
after define interface,velocity,spotweld and ....
then in Hyperview ,show the result.
my problem is, Before impact between door and impactor, i see some Stress on door at result.
please guide me, why I see stress in Door Mesh before impact?
Bestregard
Answers
-
Hi,
the stress on the door before the impact is because too high mass scaling is used; the imposed timestep increases the total mass by 633% (check the DM/M or mass error in engine out file), while the recommended is less than 2%.
There are several other issues in your model:
-the begin card declares unit system of kg m s, but material and model dimensions are consistent with tonne, mm, s.
-the initial velocity of the pole is 200- if the units are m/s it means 720 km/h! The pole impact is performed at 32 km/h.
-the pole is deformable with added mass applied on it. The computationally more efficient approach would be to put a rigid body on the pole and add mass to this rigid body.
-there are initial contact penetrations. Remove them in Hypercrash: Quality>Check all Solver Contact Interfaces or in Hypermesh: Tool>penetration check. If penetrations are less then 1/3 of the gap the Inacti=5 or 6 can be used.
-the pole could be moved closer so the impact happens sooner0 -
thank you very much
0 -
my Dear,
I have 2 question.
1) in my Model , mean Mesh size 7mm , Density : 9.85E-9 ton/l , E=210000 Mpa, i want to calculate Nodal time step by this equation: tn =L/(E/Density)^0.5
But i don't know , How to choose the right unit?
2) if after check Out file, and see increase %ERR= - 99% , is that simulation is good or bad?
I attached two different Out file,Please checked and guide me.
best regards
0 -
0
-
Glad to help.
1. Actually the formula for nodal timestep is:
Δtnodal=√2mkWhere m is Nodal mass and k is Equivalent nodal stiffness
Regarding units, just follow a consistent set:
https://www.altairuniversity.com/wp-content/uploads/2012/04/Student_Guide_55-57.pdf
For timestep calculation refer to:
III_Considerations about Time-Step - Altair University
You can review the nodal timestep in the starter out file. Initial Added mass estimation is also printed in starter out file:
2. %ERR= - 99% is not acceptable and means the simulation is diverging and the negative energy means it is dissipated. Energy error debugging:
· Check the last animation file (written before the computation stops with option /STOP in the engine file).
· Usual issue :
· Imposed time step too high
· Material badly defined
· Elastic material with large deformation
· Contact interface (stiffness, gap, contact penetrations and intersections) not correctly defined
In your case the imposed timestep is too high again: see last column mass error- it should be below 2e-2 (2%), but you have 1 (100%) and 194 (19400%) mass added
You may find helpful Free eBook: Introduction to Explicit Analysis with Altair RADIOSS. I have recently revised the third edition which should be available in the near future.
0 -
You explained so easily.
thank you very much
0 -
Hi my friend
With your good help I was able to solve Mass Err.
But there is still a fault with the energy error(ERR= -99%).I changed some parameter in my model(Contact,Material , ...).However, as soon as a collision occurs, the amount of energy increases.If possible, please guide me to fix this issue.
Is there an educational film about this?
Best regards and I hope to meet my good friends in the future.
0 -
0