we are not explicitly setting a minimum value for ENB, but in the damage evolution, we make sure that the failure strain (eps_f) is a certain multiple of the strain at damage initiation (eps_0) to prevent a snap-back behavior. So basically we would compute the failure strain based on the given fracture toughness, but if it is not big enough we would set it to
eps_f = gamma * eps_0
We use the following gamma-values:
fiber tension: gamma_a=1.1
fiber compression: gamma_kink=1.1
matrix failure: gamma_mag=2.0 (<--- this is the factor of 2 you are seeing)
best regards,
Stefan
P.S.
This is a similar approach to MAT_138 (see Keyword Manual Volume II, Figure M138-2), where L/u are relative displacements and not strains, but basically L=eps_0 and u=eps_f. And the error check described in Remark 5 says, that we need u/L to be larger than 1 (this is the gamma I was using above).
On 6/11/21 6:56 AM, LST Technical Support wrote:
I have one more question from xxx regarding MAT_261 this time. Does the model assume a minimum value for the fracture toughnesses. If so, what is this minimum value for ENB? I'm attaching a test input of a single element subjected to tension along the transverse direction and the corresponding force-displacement plot if ENB is left equal to 0.0. It seems the displacement at failure is 2 times the displacement at the peak strength.
ak
_______________________________________
RE: Changes to mat 261
there was a tiny bug in the extrapolation of the curve (LCSS) values. I have fixed this in [dev/148228, R12/148229].
[Doesn't affect any other curves or LCSS as a table.]
Stefan
Art. 68 of
Ticket#2020032510000025
-------------------------------------------------
Thanks for preparing this test case including the pcom file. I could verify what xxx and you were noticing and it seems as this particular behavior might be due to some special combination of failures of IPs, having multiple tshells throught the thickness, ... whatever. To make sure, the final stress state is within the allowable limits, I added a check and a modification of the damage values accordingly. I must admit, that I am currently not 100% convinced, that this is the right way to do, so I only put it in the DEV version for now (r146991). Please let xxx know and let them test it in additional models. If they experience any strange behavior compared to prior versions, please let me know.
Best regards,
Stefan
Am 15.04.2020 um 17:11 schrieb LST Technical Support:
xxx keeps coming back with new test cases and questions regarding mat 261. I've taken their most recent test case and cleaned it up a little (rev.k). A LS-PrePost command file (pcom) is attached which will read d3plot and produce history plots of:
1. maxima of x-stress over all the parts (fiber tension)
2. maxima of y-stress over all the parts (matrix tension)
3. minima of x-stress over all the parts (fiber compression)
4. minima of y-stress over all the parts (matrix compression)
In the mat 261 input, we have ...
XT=3000
YT=200
XC=2000
YC=8000
CMPFLG is set to 1. Under any circumstance, should I expect to see the max value ...
- in the first plot to exceed 3000? (I do. See smp1.png.)
- in the second plot to exceed 200? (I do. See smp2.png.)
... or see the min value ...
- in the third plot to be less than -2000? (I do! See smp3.png.)
- in the fourth plot to be less than -8000? (I don't. That's good, I think. See smp4.png.)
I hope my line of questioning makes sense. I want to know if you have any explanation for the "overages" seen in the first three plots.
I ran both MPP d dev 146575 (1 core) and SMP d dev 146474 (ncpu=-4). The results shown come from the SMP run.
MPP results are not identical to the SMP results, but they're close. I'm not too concerned about the differences between SMP and MPP.
jd
Ticket#2020032510000025
____________________________________________
Some general notes, examples, and references on composites in LS-DYNA are provided in the text file http://ftp.lstc.com/anonymous/outgoing/support/FAQ/composite.models
The following references are more specific to mats 261. I haven't reviewed these references in any detail so I don't know the degree to which test procedures for material characterization are addressed.
Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for
laminated fibre-reinforced composites with emphasis on fibre kinking: Part I:
Development”, Composites Part A, Vol. 37, 63-73 (2006).
http://ftp.lstc.com/anonymous/outgoing/support/PAPERS/pinho_et_al_partI.pdf
Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for
laminated fibre-reinforced composites with emphasis on fibre kinking: Part II: FE
implementation”, Composites Part A, Vol. 37, 766-777 (2006).
http://ftp.lstc.com/anonymous/outgoing/support/PAPERS/pinho_et_al_partII.pdf
Puck, A., Kopp, J., Knops, M., “Guidelines for the determination of the parameters in
Puck’s action plane strength criterion”, Composites Science and Technology, Vol.
62, 371-378 (2002).
The thesis in http://ftp.lstc.com/anonymous/outgoing/support/PAPERS/pinho_phd.pdf
is provided in lieu of adding mat 261 to the Theory Manual.
You'll find others by searching on Pinho, and mat_261 at www.dynalook.com.
jd
Ticket#2020010810000105
______________________________________________
Handwritten notes on strain rate averaging in mat 261 (and other select material models) are in
morefaq (see http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/strainrate_averaging_mats34.54.58.261.262.pdf).
This comes from Ticket 2018012310000126, Stefan Hartmann.
(Note: What look like "^"s are actually "1"s.)
_______________________________________________
yes you are correct. LCSS is the shear curve that is used for the iteratively solve for the initial fiber missalignment angle (theta_i). I have attached the two papers, that are the theoretical source for MAT_261. In the first part you may have a look at page 68 (equations 20-29) and in the second part at page 768 (equation 8) to get an idea. Maybe the curve definition in their model is "very" non-linear and therefor the iterative process to solve equation 8 in the second paper fails?
Best regards,
Stefan
On 5/20/19 8:37 PM, LSTC Technical Support wrote:
> Can you help explain MSG_SOL+1194?
>
> It seems clear that a value for theta_i could not be determined iteratively solved during initialization, and I'm guessing the shear curve mentioned in the warning is LCSS. Is that correct?
>
> Do you have any ideas on what might be wrong?
>
> Ticket#2019052010000088
>
> Hi Support,
>
> One of our clients is getting the following message in one of his models regarding MAT_261:
>
> “Part ID = 2 no convergence for thetai in MAT_261
> check shear curve! - thetai = 2.0° will be used”
>
> Do you know what the message means? Have you got any guidelines on how to sort the problem out?
____________________________________________________________________
List of additional mat 261 enhancements as described in Ticket#2018082710000204 (pdf provided) is
being tackled by John Zhao.
9/18/18
______________________________________________________________
RE: new mat 261 feature for residual strength
added feature in r129470 (trunk)...
You can now set a limit damage value for the reduction of the stresses by setting this in the flags DAF, DKF, DMF.
For example, if you set DMF=0.95 then the stress reduction depending on a matrix damage will be limited to
sig_dam = (1-min(dmat,0.95))*sig_undam
This is now possible for fiber tension (DAF), fiber compression (DKF) and matrix damage (DMF).
Furthermore, these flags were used to indicate whether the individual damage value shall decide to trigger an integration point to be failed. This is still valid, i.e.:
DAF:
.le.0: IP fails if any damage variable reaches 1.0
.gt.0: no failure due to fiber tensile failure
and you could even define DAF=-0.95 meaning, that you would tag the IP to be failed if any damage variable reaches 1.0 but still limiting the stress reduction to a certain amount.
Ticket#2018060610000104
___________________________________________________________________
RE: Normalization
he is talking about the original Paper form Pinho where he uses different characteristic lengths depending on the failure criteria (L_mat, L_kink, L_a). Honestly, I do not know if this makes really any difference ... and yes your customer is right, as we use only one characteristic length in LS-DYNA for all failure criteria.
Stefan
To: LSTC Technical Support
Subject: RE: [External] Re: MAT261 T-Shell vs Solids
Date: 2018-08-17 13:16:48
the normalizing factor in the original model is based on orientation of fracture plane in the fiber and matrix directions, this in general does not coincide with LSDYNA’s normalizing factor which is based purely on numerical aspects (for example Vol/max.AREA for solids, 1.12sqrt(Area) for T-Shells). The user thus has to be careful and must calibrate his energy release rates to account for these difference.
No action is required from your side, but the user has to be aware on how to calibrate the energy release rate parameters
Regards,
xxx
For Tshells, the characteristic length for the regularization is:
1.12 * sqrt(AREA)
so the thickness is not taken into account.
jd
Ticket#2018080910000033
____________________________________________________________________
Many thanks for the feedback, this confirms by thoughts on MAT_261/262. I’ve found that for non-crimp fabrics both material models work well as they are akin to multi-directional continuous UD layers, whereas the bi-axial woven (where the warp and weft yarn directions are both reinforcements) presents a limitation of the model.
Thanks again for your assistance and advice.
Kind regards,
xxx
Hi, xxx
I spoke to the developer of mat 262 and he had the following to say.
"MAT_261/262 are not really meant to be used for woven composites. The failure criteria for both of these models assume a rather pronounced orthotropy ... I am not finding the correct words to describe, but essentially, these models were developed for modelling endless fiber reinforced plastics. In these criterions, XC/YC as well as XT/YT have totally different meanings and cannot be interchanged without getting different responses.
So to make this short:
If they want to use M261/262 for woven fabrics, I would suggest to model the woven structure by using various UD-layers, stacked in different directions. Within one layer, the mentioned material models are not suited for woven stuff."
Ticket#2018080710000073
________________________________________________________________________
RE: Card 7 (crashfront, Puck) - mats 261 and 262 both include this card.
------------------------------------------------------------------------
r89284 | stefan | 2014-05-07 03:24:54 -0700 (Wed, 07 May 2014) | 3 lines
Changed paths:
M /ls971/trunk/dyn1.F
Not for release notes:
Fixed bug in reading SOFT (crashfront) parameter for *MAT_261/262
and
------------------------------------------------------------------------
r101548 | stefan | 2015-09-28 00:49:49 -0700 (Mon, 28 Sep 2015) | 4 lines
Changed paths:
M /ls971/trunk/dyn1.F
M /ls971/trunk/dyn2.F
M /ls971/trunk/init_once.F
Not for release notes:
fixed initialization bug for crashfront algorithmn in Mat_261.
--------------------------------------
I believe PFL applies only to shells and tshells, that is, element formulations that have a definite thickness direction and which have a user-specified number of integration points (NIP) through the thickness. I made no verification that PFL is ignored for solids, but I can't imagine that it would apply to solids.
jd
Ticket#2018041710000089
___________________________________________________________________
RE: SIGY in mat 261
Is SIGY used in damage or failure calculations?
There does not appear to be any effect in our simulations when changing the value of SIGY for shear response.
Since a non-linear shear stress-strain curve is provided, it is not clear what effect SIGY has on element response, or if this value is ignored.
ANS:
"if I have it right, the question concerns SIGY when defining a curve for the non-linear shear-stress vs. shear-strain behavior. If they use this 1D-plasticity model just with isotropic hardening BETA=1.0 then the value of SIGY will not matter. Once they have mixed or kinematic hardening (BETA=0.0 .... 0.99), the SIGY is necessary to define the "elastic" range (Sig_el in the attached figure)."
Stefan
Ticket#2018041710000089
____________________________________________________________
RE: EFS in mat 261 (both shells and solids; extracted from dev source code on 4/2018)
The variables d1tot, d2tot, ... are the total strains in the local 1-direction, 2-direction, ....
this effective strain measure to finally get rid of an element has been introduced a long time ago in MAT_54. After that it has been requested by customers to add it to MAT_58 and MAT_261/262. All of these material models use some kind of failure criterion that only take the in-plane stresses into account (sig11,sig22,sig12), even if it is used for solids. So my guess is, that due to the "plane-stress" failure criterion, the effective strain for element deletion uses in-plane strains only, even for solids.
Stefan
On 07/27/2018 08:16 PM, LSTC Technical Support wrote:
Hi, Tobias and Stefan.
Does it make sense that the effective strain effstrn (used in comparing to EFS) is calculated the same for solids as it is for shells? (Note that d1tot5 and d1tot6 are not used in calculating effstrn for solids.)
The customer has not as yet raised that question.
jd
Ticket#2018060610000113
Here's a snippet of the source code that shows how EFS in mat 261 is calculated for both shells and solids. The variables d1tot, d2tot, ... are the total strains in the local 1-direction, 2-direction, ....
c effective strain calculation...
c
c ... EFS>0: incompressibility assumption (old)
if (iefs) then
if (erodefl.ge.0.0) then
do i=lft,llt
facsa=0.5*(d1tot(i)+d2tot(i))
facsb=0.5*(d1tot(i)-d2tot(i))
facscc=facsb**2+d4tot(i)**2
effstn(i)=1.1547*sqrt(3.0*facsa**2+facscc)
enddo
c
c ... EFS<0: nearer to real effective strain (new)
else
do i=lft,llt
facsa=0.5*(d1tot(i)+d2tot(i))
facsb=0.5*(d1tot(i)-d2tot(i))
facsc2=sqrt(facsb**2+0.25*d4tot(i)**2)
facs5=facsa+facsc2
facs6=facsa-facsc2
effstn(i)=sqrt(2.0*(facs5**2+facs6**2+d3tot(i)**2)/3.0)
enddo
endif
endif
------------------------------------
r98991 | tobias | 2015-06-29 02:06:10 -0700 (Mon, 29 Jun 2015) | 6 lines
Correct the computation of effective strain for options
ERODS<0 in *MAT_058 and EFS<0 in *MAT_261 and *MAT_262.
The shear strain term was twice the size as it should have been:
sc2=sqrt(sb**2+d4tot(i)**2) --> sc2=sqrt(sb**2+(0.5*d4tot(i))**2)
Ticket#2015062510000164
______________________________________________________________________________
RE: Initializing mat 261
The initial_stress capability is supposed to work for MAT_261 as it should work for other materials as well. The problem here is, that the stress update is different than most of the material models in LS-DYNA, i.e.:
most mat-models do something like this:
sig_n+1 = sig_n + delta_sig_n+1
mat261 basically does this:
sig_n+1 = C_n+1 * eps_n+1
so it uses the total strain accumulated over time multiplied with the appropriate stiffness (maybe damaged) in there. So if you just intialize the sig_n then this would not have the expected effect. If you would like to do stress initialization with mat261, you basically would need to initalize the total strains. This would require to write out more history variables, i.e.
#31 : d1tot - total strain in 11-direction
#32 : d2tot - total strain in 22-direction
#33 : d3tot - total strain in 33-direction
#34 : d4tot - total strain in 12-direction
#35 : d5tot - total strain in 23-direction
#36 : d6tot - total strain in 31-direction
all given in the material-coordinate system.
Stefan
Ticket#2018041310000078
_____________________________________________________________
Re: characteristic length
For Tshells, the characteristic length for the regularization is:
1.12 * sqrt(AREA)
so the thickness is not taken into account.
Ticket#2018080910000033
-----------------------------------------
yes we use the same characteristic length that is used for time step calculation, so for solids: ve/Aemax and then yes, we do the regularization for each element and always using its own characteristic length.
stefan h
On 02/17/2018 12:58 AM, LSTC Technical Support wrote:
Hi, Stefan.
See the customer's question about the definition of characteristic length as it applies to mat 261. I suppose characteristic length for various element types should be defined in the Manual. Is it the same as used for time step calculation ("Time Step Calculations" in the Theory Manual), in which case I suppose the characteristic length for shells would be affected by ISDO in *control_timestep.
Ticket#2018021610000111
______________________________________________________
RE: Angles in mat 261
The misalignment angle "theta_i" is mentioned in the supporting references for mat 261, but not in the LS-DYNA User's Manual itself.
The initial misalignment angle is not a direct input parameter, rather it's iteratively solved for during initialization.
The current value of the misalignment angle is stored as history variable #8. Can enlighten us as to your interest in knowing this value? Perhaps we should consider adding HV #8 to the table of mat 261 history variables already in the User's Manual.
According to Stefan, initializing HV #8 in *INITIAL_STRESS_(SOLID,SHELL,TSHELL) serves no purpose since
the initial misalignment angle will be recalculated from the material properties anyway.
jd
Ticket#2018060610000113
-------------------------------------------------------
Misalignment angle "theta_i" as mentioned in the literature (but not the User's Manual):
As for the initial misalignment angle:
Yes this, angle is no direct input parameter and it has to be iteratively solved during initialization, depending on the stress-strain relationship in in-plane shear (at least I remember something like this), so yes it is calculated and used in the material model. I think for the user it is not very important to spend time to worry about this angle.
HV #8 is the misalignment angle, but I still would not put it in the manual as I think it
is not important for the user to look at this. If it is in the manual, I guess that people
starting to ask about this value and its meaning and so on
Stefan
Ticket#2018031210000081
history variable 49 is the misalignment frame orientation θ, which according to the Pinho reference,
is defined as the sum of an initial misalignment angle theta_i with the shear strain in the initial misalignment frame, gamma_mi.
jd
----------------------------------------------------------------------
The two angles in Figure M261-1 can be post-processed and they can be found here:
THETA is written to history variable #49
PSI is written to history variable #50
The stress at compressive failure is not stored, but recomputed each time.
ts
History variable #12 gives the computed angle of the fracture plane is using the PUCK criteria. This PUCK criteria is only implemented as a post-processing result. This PUCK criterion is not used at all in the formulation, but it was requested by Daimler at that time to have the possibility to compare the actual implementation with the criterion from PUCK. This is only activated when setting the parameter PUCK (Card 7, col 6) in the keyword card to 1. (so #12 does not correspond to ANY angle in Figure M261-1)
So now to the requests:
The two angles can be post-processed and they can be found here:
THETA is written to history variable #49
PSI is written to history variable #50
the stress they are requesting for is not stored but recomputed all the time.
Stefan
For my clarification, which angle in Figure M261-1 corresponds to History Variable #12?
ts
Ticket#2018020510000168
__________________________________________________
See example ~/test/mat261/1ele_tot.k
_______________________________________________________________
*mat_261 or *MAT_COMPOSITE_LAMINATED_FRACTURE_DAIMLER_PINHO and *mat_262
or MAT_COMPOSITE_LAMINATED_FRACTURE_DAIMLER_CAMANHO were presented at the
11th German LS-DYNA Forum, Ulm, Germany, October, 2012.
Attached are my notes taken from an abstract plus several references for
the two new composite materials. I have included these into my Guidelines
and References document.
(~/test/mat261/mat_261_and_mat_262.doc)
*mat_261 was originally incorporated through an user-defined (*mat_041)
back in 2006 (the primary references). The *mat_262 work was originally
done back in 2007.
JK
11/1/12
________________________________________________________
Author: Stefan Hartman
Date: 2017-10-02 10:05:45 -0700 (Mon, 02 Oct 2017)
New Revision: 8986
Modified:
trunk/Vol_II_Materials/MAT_261__MAT_LAMINATED_FRACTURE_DAIMLER_PINHO.docx
trunk/Vol_II_Materials/MAT_262__MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO.docx
Log:
Add description for Table definitions for fracture toughnesses
[Above documentation came late. R10 has the following release note...
*MAT_261 - *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO:
*MAT_262 - *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO:
- Allow table input for fracture toughness values for mats 261/262..
Table represents fracture toughness vs. element length vs. strain rate
(shells, tshells, solids)]
------------------------------
no, I do not have any test case for this available. This was a request by xxx and I do not know if they are actually using it or not.
Stefan
Am 05.10.2017 um 19:17 schrieb Juan Pu:
I searched through QA test cases, did not find any case with negative ENKINK or GXC for mat 261, mat 262.
Juan Pu
On 10/05/2017 09:19 AM, LSTC Technical Support wrote:
Hi, Stefan.
Sorry to bother you again. Do you have a sharable, QA test case for these new R10 table options in mats 261/262? (Or did you already provide such an example to Juan?)
Juan,
The new options for mat 261 is invoked by defining table(s) corresponding to negative values of ENKINK, ENA, ENB, ENT, and/or ENL.
Similarly, the new options for mat 262 is invoked by defining table(s) corresponding to negative values of GXC, GXT, GYC, GYT, GSL, GXCO, and/or GXTO.
jd
Ticket#2017092910000013
________________________________________________________
RE: Strain rate
As material 261 is orthotropic, three different strain rate measures are used:
e_aa_dot: strain rate in longitudinal direction
e_bb_dot: strain rate in transverse direction
e_ab_dot: strain rate in in-plane shear
All of these strain rates may be filtered due to DT and their values are available as History-Variables 54,55,56.
Now for LCSS, e_ab_dot is used as driving strain rate.
To efficiently access these history variables, use *DEFINE_MATERIAL_HISTORIES.
Ticket#2017011710000051
_________________________________________________________
Author: Tobias Erhart
Date: 2013-03-07 07:49:04 -0800 (Thu, 07 Mar 2013)
New Revision: 2842
Added:
trunk/Vol_II_Materials/MAT_261__MAT_LAMINATED_FRACTURE_DAIMLER_PINHO.docx
trunk/Vol_II_Materials/MAT_262__MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO.docx
Modified:
trunk/Vol_II_Materials/APPENDIX_A_ALPHABETIZED_MATERIALS_LIST.docx
trunk/Vol_II_Materials/MAT.docx
trunk/Vol_II_Materials/MATERIAL_MODEL_REFERENCE_TABLES.docx
trunk/Vol_II_Materials/file_list.txt
trunk/Vol_II_Materials/mtable.txt
trunk/Vol_I_Keyword/REFERENCES.docx
Log:
Add two new materials, MAT_261 and MAT_262.