Jump to content

# 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

#### Share this 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

#### Share this post

##### Share on other sites

thank you very much

#### Share this 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

##### Share on other sites

sorry, I forgot to send the files

#### Share this 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:

For timestep calculation refer to:

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.

#### Share this post

##### Share on other sites

You explained so easily.

thank you very much

#### Share this 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

##### Share on other sites

Model with Impactor(Rigid wall)

## Join the conversation

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

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.

×

×
×
• Create New...