Jump to content
Sign in to follow this  
Korosh

fake Stress in Hyperview

Recommended Posts

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

FR_Door_LH_98_11_19.hm

Share this post


Link to post
Share on other sites

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 sooner

 

FR_Door_LH_98_11_19_edit.hm

Share this post


Link to post
Share on other sites

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

Share this post


Link to post
Share on other sites

Glad to help.

 

1. Actually the formula for nodal timestep is:

Δtnodal=2mk

Where 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:

8f463b80afef8461af97eb889aee5f6736edc29d.jpg?image_play_button_size=2x&image_crop_resized=960x540&image_play_button=1&image_play_button_color=7b796ae0

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:

image.png.c50c57c50854c4513ad0ec5dcf06b5e4.png

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.

 

Share this post


Link to post
Share on other sites

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.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Sign in to follow this  

×
×
  • Create New...