Author: stefan Date: 2022-12-20 00:27:06 -0800 (Tue, 20 Dec 2022) New Revision: 15418 Modified: trunk/Vol_II_Materials/MAT_058__MAT_LAMINATED_COMPOSITE_FABRIC.docx Log: Add Tshells (ELFORM=3,5,7) ________________________________________ RE: Strain rate dependence and negative values of EA,EB,GAB I've made some improvements to the model. This "rev2" of the model is attached. The changes are summarized as follows: $ shell type 16 with hourglass type 8 $ no NLOC; put shell nodes at midplane $ SHRF=1.0 (not 0.833, which would apply to a single layer of non-composite shells) $ LAMSHT=3 $ stiffness damping on shells $ part 4 solid fully-integrated since only 1 element thru thickness $ comment out all CONTROL_CONTACT except ignore=1 and ssthk=1 $ fix scale factor on load body to represent gravity $ set VDC=0 for tiebreaks (VDC makes tiebreaks noisy in freefall test case) $ set SOFT=1 for tiebreaks $ use seg sets with proper segment orienation for tiebreaks $ XXX run only 3000 steps while debugging $ big key seems to be setting contact thicknesses or SSTHK=1 in control_contact $ add intfor for slave side of tiebreaks to check for damage ("contact gap" in intfor) $ add matsum and sleout output files I ran this model using both MPP d dev and SMP d dev, and the results are in good agreement both visually and on the basis of internal energy, kinetic energy, and velocity time history of the projectile. The primary differences I'm seeing between MPP and SMP are: - The energy ratio gets as high as ~1.25 in MPP, but returns to a more reasonable value of ~1.07 by calculation's end. This energy excursion is related to a higher contact energy in MPP. - By fringing "contact gap" from the intfor output, I can see much more tiebreak damage occurring in SMP than in MPP, but that damage is limited to the outer edges of the shell plates. jd 5/22/20 Ticket#2020041610000166 -------------------------------- I have just added a check for the load-curve ranges if used for EA or EB. For GAB, we are only using positive ranges as we assume the behavior to be the same for positive or negative shear. So if the load-curve is not defined at least in a range of -5% to +5% strain, there will be an error message. Stefan 4/22/20 Ticket#2020041610000166 ----------------------------------------- See hand-sketched explanation of DT values in strainrate_averaging_mats34.54.58.261.262.pdf In this, Stefan's "1"s looks like "^"s. ------------------------------------- Author: jday Date: 2020-04-21 08:16:10 -0700 (Tue, 21 Apr 2020) New Revision: 12124 Modified: trunk/Vol_II_Materials/MAT_058__MAT_LAMINATED_COMPOSITE_FABRIC.docx Log: 1. In description of curve option corresponding to EA,EB < 0, added the words to the effect that negative data points correspond to compression and positive data points to tension. 2. Added remark addressing which strain rate values are used for rate dependent properties. 3. Clarified last sentence in remark explaining FS=-1. Ref: Ticket 2020041610000166 Also updated history variable table at https://www.dynasupport.com/howtos/material/history-variables on or around 4/20/19 to include all the strain rates for shells and solids. Added a remark that strain rates are the smoothed values. jd --------------------------------------- When you plot some time histories of HVs 20,21,22,23 are the curves noisy? What are the peak values of strain rate seen in those plots? Your curves with strain rate on the abscissa only have 2 points where the 2nd point corresponds to a strain rate of 16.9. For any of those curves that have a negative slope, you might be in trouble if the actual strain rate exceeds 16.9 since curve data will be extrapolated. Better to add a third point to those curves so the final slope of the curve is zero. I hope the logic of doing that is clear. jd Ticket#2020041610000166 __________________________________ RE: Material orientation in shells The main thing to know for a warped shell is that the shell normal is calculated as the cross-product of the shell diagonals. That normal determines the shell plane. The element x-direction is the projection of the N1-N2 axis onto the shell plane. After that, Remark 3 on "Material Directions" under *MAT_002 in the User's Manual applies as usual. Here's an excerpt from Remark 3 which discusses the in-plane angle that goes into defining the initial material orientation at an integration point ... phi-i = beta + beta-i ... Alternatively, material orientation for mat 58 shells may be initialized by setting q1 (cosine(alpha)) and q2 (-sine(alpha)) using *INITIAL_STRESS_SHELL, in which case all the material-orientation-related input in *MAT, *ELEMENT_SHELL_BETA, *PART_COMPOSITE/*SECTION_SHELL is ignored. These history variables can be included in dynain via *INTERFACE_SPRINGBACK_LSDYNA. INN in *CONTROL_ACCURACY plays a role when using this alternative since INN affects the element's reference axis. Alpha is the angle between that element reference axis and the material a-axis. So really, alpha and phi-i are two different things. A pdf is attached that attempts to explain INN. I don't know if that helps or confuses matters. jd Ticket#2020042010000167 ____________________________________ RE: transverse shear damage the use of EPSF, EPSR and TSMD are shown in Figure M58-1 under MAT_58, i.e. the transverse shear damage evolves linearly between EPSF and EPSR. ----------------------------------- 1. we compute the effective transverse shear strain with: epseff56=sqrt(d5tot**2+d6tot**2) 2. If epseff56.le.epsf: Nothing (still elastic) 3. If epseff56.gt.epsf: Compute damage variable: dmg56=min(tsmd,max(0.0,(epseff56-epsf)/(epsr-epsf))) --> just a linear damage evolution like described in the manual which is limited by TSMD 4. Reduce transverse shear stresses: sig5 = (1-dmg56)*sig5 sig6 = (1-dmg56)*sig6 So it is quite simple. The transverse shear stresses are computed elastically, and once the effective transverse shear strain reaches the limit strain epsf, we compute a damage variable based on a linear damage evolution defined between EPSF and EPSR. Stefan On 6/26/19 1:48 AM, LSTC Technical Support wrote: > Stefan, > > Would you be able to send a description of how transverse shear damage is calculated using EPSF and EPSR? This use is already familiar with this document: > > http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/M58_Theory.pdf > > ub > Ticket#2019062510000166 _________________________________________ Author: stefan Date: 2019-02-19 06:39:57 -0800 (Tue, 19 Feb 2019) New Revision: 10852 Modified: trunk/Vol_II_Materials/MAT_058__MAT_LAMINATED_COMPOSITE_FABRIC.docx Log: Added LCDFAIL in Card 5 Column 8 Gives failure strains in each direction. Applies to both shells and solids. ____________________________________________________________________ Comment # 4 on bug 15142 from Stefan Hartmann I have fixed this issue in R10, R11 and Dev (r132875 - r132877) Am 04.12.2018 um 01:24 schrieb LSTC Technical Support: > Stefan, > > Could you please take a look at the attached file. It shows a strange deformation when using mat ID 1 or 5 in PART_COMPOSITE_TSHELL, but runs as expected when using mat ID 2. > > ub > Ticket#2018120310000189 ______________________________________________________ RE: damage in mat 58 To get an idea of how tensile fiber stress, r1 (threshold vale), and w1 (damage) interrelate, run http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/allin1_ortho_fail-in-compression_a_direction.k and plot a time history of x-stress for element 58 in one window and plot time histories of HV#1 (w1) and HV#4 (r1) in another window. Compare the curves in the two windows. (Next section addresses meaning of damage values written as HV 1,2,3. This information is repeated later, but not as concisely.) Refer to the paper  "Crashworthiness Analysis with Enhanced Composite Material  Models in LS-DYNA - Merits and Limits", 5th International LS-DYNA User's Conference", K. Schweizerhof, et al.,  located here...  http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/crash_composites_paper.pdf . It's my understanding that the material model described as "58a" in the paper corresponds to FS=0, "58b" to FS=1, and "58c" to FS=-1. Whatever the value of FS, I believe extra history variables 1,2, and 3 for mat 58 are: w1 :  damage parameter for the first local inplane direction w2 :  damage parameter for the second local inplane direction ws : damage parameter for shear in the local 1-2 plane The damage parameter is equal to (1 - exp[...]) where exp[...] is the exponential term in Eq. 5 shown on p. 12 of 21 of the  paper.  Be sure to apply the following  corrections to the Schweizerhof paper: 1. There are two negative signs in the exponent in Eq. 5.  Only one negative sign  is needed as the exponent is supposed to be negative.  Also, the condition on beta should be beta  > 1 and not b > 0. 2. The multiplier at the tail end of Eq. 5 should be written as (epsi * Ei), not epsi/Ei. 3.  Figure 2:  Caption should read "..., (b) DFAILT = 0.03" The damage parameters are perhaps written more clearly in http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/M58_Theory.pdf . "e" with no subscript is exp(1.0), that is ~2.71. The possibility of a divide by zero is eliminated in the material subroutine by calculating m11,t as 1/ln[ max( 1.1, E11T*EA/XT)] . The other m values are calculated in similar fashion. Note m = 1/ln(beta) where beta is the variable used in Eq. 5 of the Schweizerhof paper. Note there is input variable beta for the material model and beta only appears in the paper. In the model you will need to set the strain (e.g.,E11T) at which the stress shall reach the maximum (e.g., XT). This strain has to be larger than the elastic strain given by XT/EA. In LS-DYNA there is a minimum value that says: E11T.ge.max(E11T_input, 1.1*XT/EA). Internal note: Regard direct input of m-values (as mentioned in notes below)... this is an undocumented feature and should probably be avoided. Rather we ecommend the user to use positive values to set E11T, .. Ticket#2016112910000127 _______________________________________________________________________ Comment # 4 on bug 10714 from Stefan Hartmann I have implemented the MAT_58 capability for solids. It is available in trunk-version, r130659 and later. So far there is the basic MAT_58 capability with constant stiffnesses and no strain-rate dependent variables. The manual has also been updated. 9/24/18 _________________________________________________________ See section 3 of http://ftp.lstc.com/anonymous/outgoing/support/PAPERS/crash_composites_paper.pdf ___________________________________________________________ RE: Missing documentation on effect of transverse strain on failure criteria. On 7/16/2018 9:18 AM, Stefan Hartmann wrote: > > I agree that the behavior is a little unexpected in the first place, and maybe we would need to update our description for the MAT_58 behavior a little bit to make it more clear? > > Taking the PDF that you have sent me (Crashworthiness ...), the actual failure criterion used are based on the threshold values (r-values). For FS=0 (Section 3, p -6-), for FS=1 (Section 3.5.1, p -10 - top) and FS=-1 (Section 3.5.2, p -10- bottom). These loading conditions are explained in a little more detail in the attached paper (Section 5). "A constitutive model for anisotropic damage in fiber-composites", Matzenmiller, Lubliner, and Taylor, 1994. > > So without going into detail here (... as I would need to study these papers in detail as well), I'll try to answer your questions: > > Question # 1: Could you please throw some light on what is causing the > X-stress in 0-deg IP#1 to drop-off before reaching the input failure stress? > > Depending on the failure criteria chosen, the effect of transverse strains is considered in the evaluation of the actual failure criteria. Therefore you will see different maximum stresses here. If you would set the poissons ratio to ZERO, you will have an uniaxial stress state there and the results will merge to be the same. > Question # 2: I have also attached stress and damage parameter histories > for FS=-1, 0, 1. Why are X-stress curves different for FS=-1 and 0? > Looks like they use the same failure criteria. > > The same basically is true here. Depending on the failure criteria, the threshold values are computed differently, leading to a somewhat different evolution of transverse strains, which then lead to a slightly different peak stress. Ticket#2018070910000268 ___________________________________________________________ Internal note: Comment # 1 on bug 13972 from Lee Bindeman 7/6/18 Here is the existing behavior that I see: For thick shells with *MAT_058, we indeed ignore the inputted value of EC. To the d3hsp file, we write instead max(EA,EB) and for the calculation of z-stress, we use min(EA,EB). Given this inconsistency, I'm not surprised that they got confused about the behavior. I just updated trunk to change this behavior. As of rev 128276, the inputted value of EC will used by thick shell elements if EC>0. If EC is left blank or a zero or negative value is input, then min(EA,EB) will be used for the stress update, which is consistent with the current behavior. The d3hsp file now writes the value that is used, either the inputted EC or min(EA,EB). When used with shell elements, MAT_058 will now always echo EC=0 to the d3hsp file since EC is ignored. Before, we were outputting max(EA,EB) which doesn't make much sense since EC is ignored. I added a remark to the MAT_058 manual page to explain how EC behaves. I consider this an enhancement so am not planing to update the other branches and consider this finished. Ticket#2017112710000111 _________________________________________________________________________________________ MAT_58 has a total-strain formulation, so it is not initializable with INITIAL_STRESS_SHELL. Ref: bug 10064 ____________________________________________________________________ See http://ftp.lstc.com/anonymous/outgoing/support/PRESENTATIONS/LS-DYNA_R800_NewFeatures.pdf, page 24 of 31. Author: Stefan Hartman Date: 2014-05-19 07:21:12 -0700 (Mon, 19 May 2014) Log: MAT_58: Possibility to define load curves for (elastic stress vs. strain) instead of constant elastic stiffnesses EA, EB and GAB For example, EA includes this description in the R8/trunk User's Manual... LT.0.0: Load curve ID or Table ID = (-EA) Load Curve. When (-EA) is equal to a Load curve ID, it is taken as defining the uniaxial elastic stress vs. strain behavior in longitudinal direction. Tabular Data. When (-EA) is equal to a Table ID, it defines for each strain rate value a Load curve ID giving the uniaxial elastic stress vs. strain behavior in longitudinal direction. Logarithmically Defined Tables. If the first uniaxial elastic stress vs. strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stressstrain curves. Likewise for EB and GAB. --------------------------------------------------- Regarding the effect on time step (forward by JK on 3/1/16): Until r85537 there was no possibility to define proper poisson's ratio for PRCA and PRCB for MAT_58 and they were assumed to be the same as PRBA. And furthermore, until that time the stiffness used for computing the speed of sound was computed as stiff = max(E1,E2,E3) not taking into account any poisson's effect Most of the anisotropic materials compute the stiffness as the maximum of the diagonal terms in the elastic anisotropic stiffness matrix stiff = max(C11,C22,C33) which takes the poisson's effect into account. So with the change in r85537 (adding PRCA/PRCB to card4, column 7/8) I changed the computation for STIFF but only if these values are set, just to make sure that older decks will not change. To make the long story short: When using the load curves I always use: stiff=max(c11,c22,c33) where as in the version with constant E values I use 1. stiff=max(E1,E2,E3) if PRCA and PRCB are not set 2. stiff=max(c11,c22,c33) if PRCA/PRCB are defined explicitly _____________________________________________________________________________________ today I have committed some changes, especially for MAT_058 (and 158) to have the possibility to define proper poisson's ratios PRCA and PRCB. They were assumed to be equal to PRBA. Althought it was possible to define PRCA and PRCB for MAT_059, they were assumed to be PRBA as well, as MAT_059 uses the same initialization routine. So with the changes in r85537, the results for older decks with MAT_059 and shells may differ, especially when looking at the internal energies. For the solid routines I would not expect any changes. As for MAT_058 and MAT_158, the results for older decks should not change but it may appear a warning message that the utilized poisson's ratio may be illegal. sh 11/21/13 Date: 2013-11-21 02:37:37 -0800 (Thu, 21 Nov 2013) Log: Add poisson's ratios PRCA & PRCB to material cards. ----------------------------------------------------------------------------- Author: sh Date: 2013-11-21 02:29:56 -0800 (Thu, 21 Nov 2013) Modified: branches/R7.1/Vol_II_Materials/MAT_058__MAT_LAMINATED_COMPOSITE_FABRIC.docx Log: Added parameter description for transverse shear damage behavior (EPSF,EPSR,TSMD) --------------------------------------------------------------------------------- Author: sh Date: 2013-09-04 01:21:19 -0700 (Wed, 04 Sep 2013) Log: added optional card 8 and 9 Strengths and associated strains given as curves with strain rate on abscissa. Three smoothing options for strain rate. In contrast, *mat_158's rate behavior is described as follows: "A viscous stress tensor, based on an isotropic Maxwell model with up to six terms in the Prony series expansion, is superimposed on the rate independent stress tensor of the composite fabric. The viscous stress tensor approach should work reasonably well if the stress increases due to rate affects are up to 15% of the total stress. This model is implemented for both shell and thick shell elements. The viscous stress tensor is effective at eliminating spurious stress oscillations." ------------ NOTES on MAT_058 ----------------- Note regarding material orientation: When using *part_composite or *integration_shell, the orientation data in the *MAT input (AOPT, associated vector(s), BETA) from the material of the first orthotropic integration point is used for all orthotropic integration points. Each integration point still retains its own orientation angle as given by card 3 of *section_shell or by BETA from *part_composite. If mat58 becomes quickly unstable, run on v. 971 which does some checking on orthotropic elastic material constants. Also, set Ec to nonzero value (affects timestep). *mat_058 input values on Cards 6 and 7 should all be positive. Shear moduli should NOT be orders of magnitude less than the E values. The following may help if instability occurs: - set ISTUPD=0 in *control_shell. - set LAMSHT=0 in *control_shell. - set INN=1 in *control_accuracy - include *damping_part_stiffness for the part (COEF=0.1) - include shell bulk viscosity by setting TYPE = -2 in *control_bulk_viscosity See ftp://ftp.lstc.com/outgoing/support/FAQ/composite.models Test models ftp://ftp.lstc.com/outgoing/support/FAQ_kw/composites/allin1*.k are illustrative as to basic composite material model behavior. A simple model which can be exercised to observe and compare behavior of various composite material models in LS-DYNA is allin1_ortho_tension_15layers.k. In this model, I've set CMPFLG=1 in *database_extent_binary so that the stresses and strains are output in the material coordinate system (longitudinal=x, transverse=y). For any chosen element, you can plot a component of stress vs. time at all through-thickness integration points simultaneously using History > Int.pt. in LS-Prepost. Some miscellaneous notes on mat_58: dam ... indicates predamage for the crashfront (stored as "eff. plastic strain" in database) History variables 1,2, and 3 are: w1 .... damage parameter for the first local inplane direction w2 .... damage parameter for the second local inplane direction ws .... damage parameter for shear in the local 1-2 plane The damage parameter is 1 - exp[] where exp[] is the exponential term in Eq. 5 of Karl's paper. (Must first apply typo corrections to Eq. 5 as described below.) Be sure and set NEIPS to 3 in *database_extent_binary in order to output w1, w2, and ws. Also set MAXINT to the number of shell integration point for which you want output. History variables 1, 2, and 3 of mat_058 are the damage parameters for each particular integration point. If you want the average value over all the integration points, click History > Element > history var#x > Surface: Average > Plot The constitutive matrix is a function of these damage parameters w1, w2, and ws. History variables 6 and 7 are q1= cos(alpha) q2= -sin(alpha) where alpha is the angle between the element coordinate system and the material coordinate system (in the plane of the shell). (rough sketch in ~/test/mat58/MatDir_q1_q2.pdf) History variable 8 is is a flag that is either equal to 1 (not failed) or 0 (failed). Except as noted below, the input strain values for mat_058 are tensorial (true) strains. The shear strain values GAMMA1 and GMS are engineering shear strains, i.e., twice the tensorial shear strain. ERODS is the Maximum effective strain for element layer failure. A value of unity would equal 100% strain. The latest version of the User's Manual states: ERODS.GT.0.0: fails when effective strain calculated assuming material is volume preserving exceeds ERODS (old way). ERODS.LT.0.0: fails when effective strain calculated from the full strain tensor exceeds |ERODS|. To elaborate just a bit: When ERODS.GT.0.0, ERODS is evaluated against a scalar strain computed from the two in-plane normal strains and the in-plane shear strain. The three values of strain that go into its computation are available for output as extra history variables 10, 11, and 12. scalar strain = 2/sqrt(3) * sqrt[ 3*((eps1+eps2)/2)^2 + ((eps1-eps2)/2)^2 + eps4^2 ] where eps1 = hist var 10 eps2 = hist var 11 eps4 = hist var 12 = engineering (not tensorial) shear strain In version 971, this scalar strain value is history variable #15. To get 15 extra history variables written to d3plot, you'd need to set NEIPS=15 in *database_extent_binary. When ERODS.LT.0.0, ------------------------------------------ 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 -------------------------------------------- abs(ERODS) is evaluated against a scalar strain that is closer to the traditionally defined effective strain which accounts for the through thickness strain and transverse shear strains. This option was added in response to the observation that history var#15 (see above) was not in close agreement with "effective strain" as plotted by LS-PrePost and this bothered some people. When the effective strain at an integration point exceeds ERODS, that integration point fails and ceases to carry stress. The element is not deleted until ALL integration points have failed. (see http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/composites/allin1_ortho_bend.erods*.k) Whether ERODS is set negative or positive, it will be in the ballpark of classic effective strain as described in the literature. My 2 cents is that a failure criterion based on any scalar strain quantity can offer only an ad hoc approximation of real failure. If you're uncomfortable with using ERODS as a failure criterion, set it to a very large value so as to disable it. There are several strain-based failure criteria you can optionally invoke using *mat_add_erosion (including the ability to erode shell elements based on max principal in-plane strain using LCFLD, Ticket#2016070410000057). Failure criteria which trigger material erosion are not true material properties in the sense that factors unrelated to the material model affect what constitutes an appropriate value for the failure parameter(s). Such factors include type of loading and mesh refinement. As such, failure parameter(s) require calibration according to the model construction and simulation conditions. In short, some calibration of model results to component tests resulting in material failure are necessary in order for reliable prediction of material failure to be possible under similar circumstances. By similar, I mean similarity in geometry, mesh density, loading conditions, etc. The 'plastic strain' stored in d3plot and elout is not a strain value at all in the case of mat_58 but rather an indicator flag for failure. If the quantity (E11C * EA/XC) is less than zero, then the input parameters on Card 6 are not interpreted as strains but are instead taken directly as the Weibull Scale Parameters (m) as defined in Matzenmiller, Lubliner, and Taylor. Relating these m values to the beta defined in Eq. 5 of Schweizerhof: mi = 1 / (ln(betai)) The source code also seems to indicate that TAU1 and GAMMA1 are used not only if FS < 0 but also if FS > 0. Corrections to the Schweizerhof paper: "Crashworthiness Analysis with Enhanced Composite Material Models in LS-DYNA - Merits and Limits", 5th International LS-DYNA User's Conference (1998): 1. There are two negatives in the exponent in equation 5. Only one is needed as the exponent is supposed to be negative. Also, the condition on beta should be beta > 1 and not b > 0. 2. The multiplier at the tail end of Eq. 5 should be written as (epsi * Ei), not epsi/Ei. 3. Figure 2: Caption should read "..., (b) DFAILT = 0.03" _______________________________________________ Based on a uniaxial compression test of mat_58: Local Eps-zz is NOT zero even ISTUPD=0 and shell thickness remains constant! (Similar for mat_59) When ISTUPD=1, shell thickness begins to reduce after stress attains SLIM value (thickness, intuitively, should continue to increase as element is being compressed in-plane). _______________________________________________ Regarding nonlinear shear behavior (active when FS < 0 or FS > 0), refer to the figure in the mat_058 section of the Users Manual. The shear stress-strain behavior is nonlinear until the point GAMMA1,TAU1 is reached and follows Eq. 5 in the "Merits and Limits..." paper by Schweitzerhof et al. but some explanation and correction of the Equation is required: - There are two negatives in the exponent in Eq. 5. Only one negative is needed as the exponent is supposed to be negative. - Also, the condition on beta should be beta > 1 and not b > 0. - The multiplier at the tail end of Eq. 5 should be written as (epsi * Ei), not epsi/Ei. - When it comes to describing the nonlinear shear behavior, subtitute the following into Eq. 5: TAU1 for sigfi GAMMA1 for epsq gamma for epsilon G for E The shear stress-strain curve reverts to a linear relationship between points GAMMA1,TAU1 and GMS,SC. _______________________________________________ If the quantity (E11C * EA/XC) is less than zero, then the input parameters on Card 6 are not interpreted as strains but are instead taken directly as the Weibull Scale Parameters (m) as defined in Matzenmiller, Lubliner, and Taylor. Relating these m values to the beta defined in Eq. 5: mi = 1 / (ln(betai)) For mat_058, the variable labeled in LS-Prepost as "plastic strain" corresponds to the variable dam(nlq). Up to 15 extra history variables can be written for mat_058. hist var #1 = w1(nlq), hist var #2 = w2(nlq), hist var #3 = ws(nlq), hist var #4 = r1(nlq), hist var #5 = r2(nlq), hist var #6 = q1(nlq), hist var #7 = q2(nlq), hist var #8 = efail(nlq), hist var #9 = r3(nlq), hist var #10 = d1tot(nlq), hist var #11 = d2tot(nlq), hist var #12 = d4tot(nlq), hist var #13 = qq1(nlq), hist var #14 = dt(nlq), hist var #15 = c11(nlq), ________________________________________________________ History variables 4, 5, and 9 remain a bit of a mystery so strike these from webpage. see Ticket#2016062010000046 6/24/16. ---------------------------------- The History-values 4,5 and 9 for MAT_058 are the so-called threshold values. These parameters indicate the stress state in the failure criterion. For example for FS=-1.0, the failure criterion in longitudinal tension would be: (sig_11/XT)^2=1 and r1=(sig_11/XT)^2 So the r1-value will be in the range between [0..1]. At the beginning it is 0, then it will grow until 1, which equals the actual reaching of the specific failure criteria and then it will decrease again due to damage evolution. The same holds for r2 and the third value r3 is only available for FS=-1. So basically the r-values describe an indicator of how far the current stress state is away from reaching the actual failure criterion. stefan 1/30/14