Car Airbag Deployment Simulation

[Vijay1988]

Hi,

I want to learn a car airbag deployment simulation using Abaqus. It would be great help if any of you please share .inp and .cae file with me if you had already worked on it.

My intention is to learn how to create an airbag model, define the required properties, inflate it using Abaqus keywords, and a dummy human head will strike against it.

I have already created an airbag and tried to inflate it with no success. I also studied the sidecurtain_airbag_fabric available for reference. But, I found it very complicated to understand.

I kindly request you to share it with me if you have already worked on it. So that I can study it and apply the same knowledge to my airbag. It will be a great help.

Thanks in advance.
Vijay

P.S With reference to thread799-249290.

Dear Akabarten,

It would be great help if you could please create a simple model and share it with me. I will highly appreciate it. Awaiting for your positive response. Thank you.

 

[akabarten]

Hi,

I have already created an airbag and tried to inflate it with no success

Could you share your inputdeck (*.inp), please?

I add example of curtain airbag from Abaqus documentation and make it simple.
1. All not airbag stuff are removed (impactor, fix frame, ...)
2. The airbag is not fold but flat.
3. It is one chamber airbag not mulitichamber
4. Does not use gas generator but the pressure is applied as boundary condition.
I think it is enough simple example to start with airbags in Abaqus.
When this model will have no secrets for you we will make it more realistic.

Regards,
Bartosz

 

[rstupplebeen]

In the example problems manual there is an example in section 3.3.2

Please see the online documentation here.

I hope this helps.


Rob Stupplebeen
OptimalDevice.com
My LinkedIn

 

[Vijay1988]

Hi Akabarten,

Thank you very much for replying. As per your request, I am sharing my .inp file.

I am getting few errors after running the .inp file in Abaqus. I am not able to solve them. Will you please run the file and see where exactly I am going wrong?

Thank you,
Vijay

 

[Vijay1988]

Hi Akabarten,

I was able to inflate my airbag. But my airbag looks like a balloon instead of an airbag. Why is it so? Does my inflator is very strong? or my airbag size is too small?

I tried to reduce the gas mass flow rate to the half, but it gave me the following error:

**The fluid inflator attached to the fluid cavity with reference node number 2715 has a negative heat capacity at constant temperature (Cv)**

What can be the possible solution for it?

Please see the attached .inp file.

Thank you,
Vijay

 

[akabarten]

Hi,

airbag looks like a balloon instead of an airbag. Why is it so? Does my inflator is very strong? or my airbag size is too small?

I guess the inflator is too strong. You have pressure around 1.5 [bar].
More realistic value for airbag will be something below 0.5 [bar].
You can control pressure value with vents. It will add gas leakage to cut down pressure.

Please keep in mind final airbag shape is not only pressure dependent.
It can be also be material orientation or straps inside the bag.

I made a package with you with some models to show the influence.

BTW: It is recommended to use three node membrane elements for airbags in Abaqus.

Regards,
Bartosz


VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Vijay1988]

Hi Akabarten,

Thank you very very much for sharing the files. It was a great help.

I reduced the pressure of my airbag and now it looks like an airbag. But at the end of simulation my airbag shrinks. Will you please check my file and let me know why is it happening so? Is it because of the leakage?

Please see the attached file.

Thank you,
Vijay.

 

[akabarten]

Hi,

Is it because of the leakage

You have no leakage, no *FLUID EXCHANGE keyword in the model.

But at the end of simulation my airbag shrinks

Your airbag is shrinking because the pressure goes down till ambient pressure value or even more (underpressure).
The reason of this is gas temperature which goes down as well.
Your temperature curve does not cover whole time of your simulation.

**
*Fluid inflator property
...
0.0396,		83.75,		0.0003275
0.0397,		83.57495,	0.0003275
**

In this case Abaqus will approximate missing values base on two last points in the curve.
But your points make decreasing slop, so you get low temperature later in simulation (low pressure), maybe even below zero.
I add one extra point to avoid temperature drop down.

**
*Fluid inflator property
...
0.0396,		83.75,		0.0003275
0.0397,		83.57495,	0.0003275
0.0400,		83.57495,	0.0003275
**

Now the temperature will be keep at 83.57495[K].
With this modification the airbag is deployed for whole time of simulation, no shrinking.

Usually massflow curve at some time is set to zero. You put the mass into the airbag for whole time.

Regards,
Bartosz


VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Vijay1988]

Hi Akabarten,

Thanks a lot. Thank you very very much. It works. You have got amazing knowledge of Abaqus. Please tell me what resources/books/websites etc. should I use to get in-depth knowledge of FEA, Abaqus like you?

You mentioned that- s recommended to use three node membrane elements (M3D3) for airbags in Abaqus. Will you please explain to me why M3D3 elements are preferred over M3D4 elements? I read that 4-noded elements give better accuracy in results compared to 3-noded elements. Because triangular elements have higher stiffness than rectangular elements hence the resulting stresses of triangular elements are lower than actual stresses.

Thank you,
Vijay

 

[akabarten]

Hi,

Please tell me what resources/books/websites etc. should I use to get in-depth knowledge of FEA, Abaqus

I wish give you simple answer but unfortunately I do not know such resources.
I think to get know Abaqus (any FEA software) well you have to start daily work with it.

Will you please explain to me why M3D3 elements are preferred over M3D4 elements

Sound silly but I do not know. I know Abaqus developer recommends use tria node membrane elements.
All airbag simulations with Abaqus are made with M3D3 elements. Quad elements are problem for fully folded airbags due to bad quality.
You have almost no option to control element quality inside folded airbag and quad elements can have extremely high warpage values.
Abaqus will rise an error about extreme element distortion and will not start analysis for M3D4 elements in this case. This is not a problem for tria elements.
I guess some developers decided to overcame a problem on element implementation level and other said "Screw it, ... let they use tria elements" ;-)
Ls-Dyna/Pam-Crash recommended to use quad membrane elements where Abaqus/Radioss recommended tria elements.

4-noded elements give better accuracy in results compared to 3-noded elements, triangular elements have higher stiffness than rectangular elements

It is true, for sure make a difference for shells where bending is calculate as well.
I guess for membrane with tension mode only this does not make such big difference.

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Vijay1988]

Hi Akabarten,

Thank you very much for answering my questions in detail. That was very nice of you. I really appreciate your time.

I am working on the 2nd part of the project .i.e to import the dummy human head into the existing airbag file.

I am planning to proceed as follows. Please confirm whether my steps are correct or need to be changed.

Step 1) Download a dummy head from Google.com and mesh it using Hypermesh.
Q1) How to decide element size and type for meshing of human head?
Q2) What are the material properties for human head?
Q3) What section should be assigned for the human head? (Solid? Shell? My downloaded human head is made of surfaces)

Step 2) Export the 'node and element' data of human head into .inp file.

Step 3) Paste the 'node and element' data of a human head into the .inp file of an airbag with an offset value?
Q4) How to decide this offset?

Step 4) Use *NMAP keyword to Map nodes from human head coordinate system to airbag and rotate, translate, or scale the nodal coordinates.

Step 5) Define the reference node for the human head

Step 6) Define the initial condition for the human head?

Step 7) Define the surface interaction and contact properties between human head and airbag surfaces
Q5) What kind of surface contact will you recommend?


Step7) Create a dynamic explicit step to strike the human head against inflating airbag

If you have any similar .inp file then I kindly request you to share with me.

Sorry to bother you so much. I highly appreciate your time and consideration.

Please help me clear my above doubts.

Thank you,
Vijay

 

[Vijay1988]

Hi Akabarten,

Looking forward to your response.

Thank you.

 

[akabarten]

Hi,

Standard approach to test airbags in simulation is to use "rigid impactor".
It can be simple shape (rectangular) or it can be simplified shape of human head (like in curtain airbag example in abaqus documentation).
In hardware those impactors usually are much stiffer compare to the airbag so in simulation they are model as rigid bodies.
In this case you do not have to take into account material data. Material property which make a different is density since it controls impactor mass.

Impactor mass and initial velocity define energy (E=(m*V^2)/2) which has to be dissipated by the airbag.
So first you have to answer for question which energy level I want to dissipate with my airbag and then choose mass and initial velocity.
It does not make a difference what you change (mass or initial velocity) as long initial energy is the same.
Keep in mind using not realistic density value can lead to unstable contact behaviour.

Q5) What kind of surface contact will you recommend?

Use general contact with default settings for start.

Paste the 'node and element' data of a human head into the .inp file of an airbag

You can think about using *INCLUDE keyword. It is easier to manage big models.

How to decide this offset?

Respect to initial velocity and time you need to deploy the airbag.
If your airbag needs 40ms to deploy and initial velocity is 6[m/s] you have 6[m/s]*0.04=0.24[m] (s=V*t).
0.24[m] is a raw distance between start point of the head and point where you expect have contact with the airbag.

Q1) How to decide element size and type for meshing of human head?
Q2) What are the material properties for human head?
Q3) What section should be assigned for the human head? (Solid? Shell? My downloaded human head is made of surfaces)

For start you can mesh it with shell rigid elements and adjust density to get the mass.

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[Vijay1988]

Thanks a lot. That is really very helpful. I highly appreciate the time you have given to write an answer and share your knowledge. Thank you again.
Vijay