Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2020-09-03 06:06:36

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Correct model for plastic material

Hi,

I'm trying to model the attached plastic material behavior (ASA). The problem is that it (like many plastics) has a multi-linear elastic AND plastic range. As far as I know, VMIS_ISOT_TRAC calculates plasticity right after the first point on the traction curve (yield). So it does not allow to model the elastic part. ELAS_VMIS_TRAC does not model plasticity. Is there any combination of both?

Another question is regarding the deformation: GROT_GDEP is only valid for small strains (<1 %?), so also not applicable. SIMO_MIEHE does not work with ELAS_VMIS_TRAC.

Is there really no way to model this curve, or am I just blind? smile

Greetings
Marco


Attachments:
stress-strain-curve.png, Size: 11.72 KiB, Downloads: 64

Offline

#2 2020-09-07 16:14:13

mf
Member
Registered: 2019-06-18
Posts: 118

Re: Correct model for plastic material

Hi,

I am not a very avid user of plastic simulation, but I am pretty sure, that this is not possible out of the box. At least I do not know about it.
Your question boils down to the very definition of elastic behaviour being the reversible (linear) first part of the curve. By the way, similar to my recent answer in post 25193, it is always a choice to make where to set zero plastic stress/strain, almost with every 'real' material (meaning with data from a stress-strain test). Real stress-strain curves are almost never really linear in the 'elastic' part of the curve, that was the reason for the invention of the proof stress in the first place (stress at 0.2% strain for example for most of the steels). But there are exceptions: for example construction steels show a really well defined linear part and yield stress. So, what you ask is pretty common, aside from the really weird shape of your curve (are all three stiffnesses really reversible?).

With VMIS_ISOT_TRAC you have three choices with your curves, depending on where you set your zero plastic strain:

1.) in the first kink, rest of the data is considered 'plastic'. Then your plastic strain will be wrong (higher). Elastic strain/stress will be correct, but only if low.
2.) in the second kink, rest of data 'plastic': elastic strain will be higher in the results for a given stress, especially when stresses are low. Plastic strain will be off a little.
3.) in the third kink: plastic strain will be correct, modulus will be wrong (lower). Thus, elastic strain will be higher for a given stress.

That is the way I see it, I could be wrong :-). Maybe a real CA expert can comment,

Mario.

Last edited by mf (2020-09-07 16:15:24)

Offline

#3 2020-09-22 13:09:03

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

Hi Mario,

thanks for your detailed answer. Let me add that the curve I use is not like in the schematic picture, where the coarse resolution implies the behavior you interpreted. Until the yield point there are more data points available for a smoother curve.

Can anyone contribute to this topic / my dilemma?

Thanks
Marco

Offline

#4 2020-09-23 06:51:46

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

Re: Correct model for plastic material

Without your command file, it is difficult to know what you are upto, but ELAS_xxx refers to elastic analysis. You should perform non-linear analysis with proper material behaviour (or Comportment in CA language) to simulate the plasticity.

Offline

#5 2020-09-23 08:41:25

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

My question is of general nature, so I did not post any comm-file.
The problem is, that there seems to be no model that accounts for non-linear elasticity AND plasticity.

Offline

#6 2020-09-28 07:12:03

cwf007
Member
From: Malaysia
Registered: 2020-06-05
Posts: 13

Re: Correct model for plastic material

Hi Marco,

Did you mean by Nonlinear elastic + nonlinear plastic material?
ABAQUS keyword: *HYPERELASTIC
NASTRAN keyword: MATS1

Im curious to know whether code_aster can cater this kind of material model too, since i will be doing alot of plastic component!


Thank you.


Warmest Regards,
cwf007.

Offline

#7 2020-09-28 11:15:26

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

yes, thats what I meant.

Offline

#8 2020-09-28 17:07:34

sb1966
Member
Registered: 2015-03-16
Posts: 180

Re: Correct model for plastic material

Hi,
I am not an expert in this field. But if you want HYPERELASTIC behaviour, there is an example of MFRONT implementation of the same. Please see
h   ttp://tfel.sourceforge.net/gallery.html#hyperelasticity (please correct in the beginning).

Hope this helps..

Regards.

Sukumar

Offline

#9 2020-10-01 06:48:45

thomas.helfer
Member
Registered: 2013-09-26
Posts: 114

Re: Correct model for plastic material

Hi,
Most finite strain plastic behaviours can be implemented in MFront and then used in code_aster.
If you have a specific set of constitutive equations you want to implement, do not hesitate to post it on the MFront forum.
Regards,
Thomas Helfer

Offline

#10 2020-10-01 08:36:41

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

Hi Thomas,

thanks for the hint regarding MFRONT, I wasn't aware of that. However I do not find myself in the position to implement new material models (or even understand the fundamentals of them) and rather have to look for existing implementations. I thought it was a very common task to model what I am looking for (non-linear isotropic elastic + non-linear isotropic plastic).

Regards
Marco

Offline

#11 2020-10-01 21:36:11

thomas.helfer
Member
Registered: 2013-09-26
Posts: 114

Re: Correct model for plastic material

Hi Marco,
Do not hesitate to show me your constistutive equations (tfel-contact@cea.fr). It shall be straightforward to implement.
Best,
Thomas

Offline

#12 2020-10-02 09:41:18

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

Hi Thomas,

thank you for this offering. However, I've done a quick look through other codes (NASTRAN, LS DYNA) codes material models available, and couldn't find this type of behavior either ... I have no overview / knowledge of the theoretical models available. Seems I was wrong about assuming this as a common model. Again, I'll attach a (better) snapshot of the materials behavior, showing the elastic and plastic regions.

Marco


Attachments:
stress-strain-curve.png, Size: 11.83 KiB, Downloads: 30

Offline

#13 2020-10-02 11:32:56

sameer21101970
Member
Registered: 2019-09-06
Posts: 246

Re: Correct model for plastic material

Mr. Thomas is right person.

Last edited by sameer21101970 (2020-10-02 12:09:02)

Offline

#14 2020-10-02 12:59:08

sameer21101970
Member
Registered: 2019-09-06
Posts: 246

Re: Correct model for plastic material

refer attachment for stress -  strain curve...it seems to be what you are looking


Attachments:
strainstress.dat, Size: 13.08 KiB, Downloads: 16

Offline

#15 2020-10-02 20:46:48

thomas.helfer
Member
Registered: 2013-09-26
Posts: 114

Re: Correct model for plastic material

Hi,

a stress-strain curve is not enough to have an idea of how to describe accuratly the material without make further assumptions.

To describe your curve, I could  assume:

- isotropy
- linear elasticity
- plasticity with the von Mises criterion and Voce isotropic hardening rule (exponential hardening rule).

See attached a package with three files:

- the MFront implementation (17 lines long)
- a unit test using MTest
- The resulting stress-strain curve

Hope this helps.

Regards

Thomas


Attachments:
Voce.zip, Size: 12.44 KiB, Downloads: 15

Offline

#16 2020-10-03 11:57:04

sameer21101970
Member
Registered: 2019-09-06
Posts: 246

Re: Correct model for plastic material

Dear Mr. Thomas,

I am super excited towards Mfront, to know more on Voce.Mfront.
I want to know how you take decision on below values R0 & Rinf and what this 2 parameters defines.
Also, if i want to start defining material laws in Mfront, what will be the correct path of learning Mfront.
Thanks

@Brick StandardElastoViscoPlasticity{
  stress_potential : "Hooke" {young_modulus : 150e9, poisson_ratio : 0.3},
  inelastic_flow : "Plastic" {
    criterion : "Mises",
    isotropic_hardening : "Voce" {R0 : 150e6, Rinf : 200e6, b : 1000}
  }
};

Offline

#17 2020-10-04 10:42:24

thomas.helfer
Member
Registered: 2013-09-26
Posts: 114

Re: Correct model for plastic material

Thanks for you interest.

The Voce.mfront file that I sent you uses the StandardElastoViscoplasticity brick (search "mfront StandardElastoViscoplasticity" in google and go the the first page, unfortunately, I can't post addresses on this forum.). This brick provides a set of predefined and composable stress criteria, isotropic hardening rules, kinematic hardening rules. The idea is to be as declarative as possible and it enables implementing behaviours without a single line of code, just like in the Voce.mfront file. The page of the StandardElastoViscoplasticity brick describes in details what is available out of the box.

For more general behaviours, have a look a the gallery (In the top menu of main page of the mfront website, go to Documentation->Gallery). It is a set of tutorials for various kind of behaviours (damage, plasticity, viscoplasticity, single crystal behaviours, hyperelasticity, hyperviscoplasticty, etc...).  Those tutorials will teach how to implement (with a superset of C++) all those behaviours using MFront. A bit more difficult than using the StandardElastoViscoplasticity brick, smile

Last but not least, you may want to give the general documentation a ride. It is mostly in French and it may sometimes be outdated (everything will work, but there may be recent developments that would be more straightforward. For example, the tutorial.pdf file will show you how to implement a viscoplastic behaviour with isotropic and kinematic hardening, which can be in most cases done much more easily using the  StandardElastoViscoplasticity brick).

Do not hesitate to contact me. (In the main menu, Getting help -> Contact)

Good luck,

Thomas

Offline

#18 2020-10-05 07:40:57

sameer21101970
Member
Registered: 2019-09-06
Posts: 246

Re: Correct model for plastic material

Very Thanks for Detail Explanation. Will Contact in case of difficulty.

Offline

#19 2020-10-14 11:23:14

marco.mueller
Member
Registered: 2020-01-16
Posts: 24

Re: Correct model for plastic material

Hi Thomas,

thanks again for your investigation here and the files. Anyway, this is not what I was looking for: A non-linear elastic region instead of the linear (Hooke). However the project is finished for the moment and I may resume here somewhere in the future.

Regards
Marco

Offline

#20 2020-10-14 11:32:21

thomas.helfer
Member
Registered: 2013-09-26
Posts: 114

Re: Correct model for plastic material

Hi Marco,
I did not have enough information on the non linear elastic part. Anyway, if you ever need this, don't hesitate to contact me.
Best,
Thomas

Offline