Files pertaining to the KCSE material *MAT_072R3/*MAT_CONCRETE_DAMAGE_REL3 are: http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/mat72r3 (a text file which you're looking at now), http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/mat_072r3.pdf , http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/mat72r3_examples_from_qa.tar.gz (examples). _______________________________________________________________ RE: Release 4 or so-called Modified K&C Model This model has not been implemented. I'm not sure it will be implemented or not. Before it can be implemented into LS-DYNA, we need the paper authors from PLAUST to provide a legal document from K&C to approve the implementation, because as you see from the name, the model is a modified K&C model. I told the authors to do so way back last year, but so far I didn't get any response. Due to the copyright issue, I think we still have to wait. Thank you, Youcai 2/27/20 Hi, Youcai. What is the status of this "Modified K&C model" as it pertains to LS-DYNA? Is it something that is worth pursuing or is Release 3 (*MAT_072R3) the preferred material model? jd Ticket#2020022610000221 Ticket includes a pdf. ___________________________________________________________________ For better understanding of *mat_072r3, See these references ... - Malvar (1996), http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/concrete.CP27_WES96K.pdf. - Schwer, L.E., and Malvar, L.J., "Simplified Concrete Modeling with *MAT_CONCRETE_DAMAGE_REL3," 4th German LS-DYNA Forum, Bamberg, Germany, October, 2005. http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/mat_072r3.pdf - "Recent Improvements to Release III of the K&C Concrete Model", Magallanes et al, http://www.dynalook.com/international-conf-2010/Simulation-1-4.pdf . - "K&C Concrete Material Model Release III—Automated Generation of Material Model Input, Malvar et al, 2000." (Contact Joe Magallanes at magallanes@kcse.com to request this one.) For further information on concrete modeling , see the files in http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete starting with the file "concrete_models_faq" ________________________________________________________________ List of pdfs in my ~/test/mat72r3 (name of paper and first author listed). Some of these are in http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete . concrete.CP27_WES96K.pdf "CONCRETE MATERIAL MODELING IN EXPLICIT COMPUTATIONS" L.Javier Malvar improved_mat72.pdf "Constitute equations for concrete materials subjected to high rate of loading" Matthias Unosson KCCM_JEngMech2.pdf "Numerical Modeling of Concrete Using a Partially Associative Plasticity Model" Youcai Wu Magallanes_et_al_2010b.pdf "FEASIBILITY STUDIES OF A PLASTICITY-BASED CONSTITUTIVE MODEL FOR ULTRA-HIGH PERFORMANCE FIBER-REINFORCED CONCRETE" Joseph Magallanes Mardalizad_Manes_Giglio.pdf "Four-point bending test on a middle strength rock: Numerical and experimental investigations" A. Mardalizad mat_072r3.generate_matl_input.pdf (not to be distrib by LSTC directly; see note above) "K&C CONCRETE MATERIAL MODEL RELEASE III—AUTOMATED GENERATION OF MATERIAL MODEL INPUT" L.Javier Malvar mat_072r3.pdf "Simplfied Concrete Modeling with *MAT_CONCRETE_DAMAGE_REL3" Len Schwer M_M_G.pdf "The numerical modelling of a middle strength rock material under Flexural test by Finite Element method-coupled to-SPH" A. Mardalizad P-14-3_validateconcretelaws.pdf "Validation studies for concrete constitutive models with blast test data" Youcai Wu Simulation-1-4.pdf "Recent Improvements to Release 3 of the K&C Concrete Model" Joseph Magallanes TR-11-36-5-KCCM.pdf "USE AND VALIDATION OF THE RELEASE III K&C CONCRETE MATERIAL MODEL IN LS-DYNA" John Crawford TR-11-36-6-KCCM.pdf (Same title, date, authors, number of pages. It appears only the document number is different.) http://ftp.lstc.com/anonymous/outgoing/support/TR-11-36-6-KCCM.pdf wu_crawford.pdf "Numerical Modeling of Concrete Using a Partially Associative Plasticity Model" Youcai Wu ______________________________________________________________ I want to understand a few things that exist in the messag file under this banner ... ------------------------------------------------------------- Updated Release III K&C concrete model by K&C/Javier Malvar (9/99 updated 4/12) based on LRDA/K&C f3dm16w.f (8/7/95) LS-DYNA Release III of Mat072 by Len Schwer (May 04) & Y.Wu (April, 12) ------------------------------------------------------------- 1) the meaning of "pressure phi" ANS: This defines the ratio between tensile and compressive meridian (refer to Eq.(20) in the attached paper). 2) the meaning of Fyc at line 183 ANS: This is an intermediate variable defined in the implementation, which is the yield strength of the concrete. 3) the meaning of Ec at line 184 ANS: This is the estimated initial Young's modulus. Another question: I can see the value of the tensile pressure cut off at d3hsp file (the value off the tensile strength that I input to the material model). I want to know if I can control (change) the value of the tensile pressure cut off and to keep the value of the tensile strength constant. ANS: The pressure cutoff cannot be input by user. Answers provided by Youcai Wu. 11/13/18 Ticket#2018060510000026 ------------------------------------------------------------- Regarding the pressure-volume response in mat 72r3, the automatically generated EOS does not include tensile data. Rather, it seems, the compressive curve is extrapolated linearly into the tension regime. The tensile pressure is limited by the tensile cutoff and/or tensile strength, which are reported in d3hsp... " tensile cutoff (max. prin. stress) = 3.186E+00 maximum failure surface a0 ....... = 1.019E+01 maximum failure surface a1 ....... = 4.463E-01 maximum failure surface a2 ....... = 2.343E-03 yield failure surface a0y ........ = 7.696E+00 yield failure surface a1y ........ = 6.250E-01 yield failure surface a2y ........ = 7.468E-03 damage scaling factor b1.......... = 1.600E+00 damage scaling factor b2.......... = 1.350E+00 damage scaling factor b3.......... = 1.150E+00 load curve for strain-rate scaling = 0. tensile strength (max ppal stress) = 3.186E+00" A small test case is attached in which a small tensile pressure is first prescribed, followed by a larger compressive pressure. The Measure>Volume feature in LS-PrePost can be used to plot volume vs. time. You can then cross-plot that volume curve with the pressure vs. time curve. jd Ticket#2018060510000026 ____________________________________________________________ (this problem was forwarded to Joe at KCSE) For my own benefit and piece of mind, I simplified your model to a single element that is compressed hydrostatically and then completely unloaded. See the attached input deck. I think the observations made using your model of a cylinder also apply to this single element model. The resulting pressure vs. volumetric strain plot is shown in the attached image. It certainly appears that the bulk unloading is linear and so there is a significant, nonzero volumetric strain (a "residual" volumetric strain) after unloading to zero pressure. Yet history variable #4, which is referred to as "plastic volumetric strain" in http://www.dynasupport.com/howtos/material/history-variables , remains zero. Perhaps Youcai is familiar enough with the mat 72r3 source code to confirm whether history variable #4 is really the plastic volumetric strain, and if so, how that quantity is calculated. ... jd Ticket#2018031910000112 ______________________________________________________________ Q: Can you the 0-1 & 1-2 Damage parameters and what those values related to in layman terms? ANS: Damage varying from 0 to 1 means the material hardens from yielding to its maximum strength. Varying from 1 to 2 means the material softens from its maximum strength to residual strength, which is usually 0 for unconfined concrete. A simple way to explain the range is: d=2x/(x+xm) when x=0, d=0, before yielding when x=xm, d=1, hardened to maximum strength when x-infinite, d=2, softened to residual strength Use can also refer to the attached paper, Numerical Modeling of Concrete Using a Partially Associative Plasticity Model, Youcai Wu and John E. Crawford Youcai Ticket#2017080910000115 _______________________________________________________________ My quick answer is your interpretation seems right. Secondly, Mat72r3 does NOT support implicit. So, user better uses for explicit calculation. Thank you, Youcai Quoting LSTC Technical Support : > Hello Youcai, > > I wonder if i could have your comment on this? The customer is in his model > (attached) restarting an analysis via a dynain file. The results between > analyses are discontinuous. (X_stress_t3.png). > > My interpretation of what is happening is as follows: > -I'm not very familiar with MAT_072R3, but understand that it internally > generates an equation of state. > -The manual says for *INITIAL_STRESS_SOLID: > "...for... material that requires an equation of state (*EOS), the specified > initial stresses are adjusted to be in accordance with the initial pressure > calculated from the equation of state." > -It seems that in this case, the above statement is holds, and that the > discontinuity is due to this initialization. > > So my questions: > 1. Does my interpretation of what is happening seem correct? > 2. Is there any way the behavior could be improved - should a restart done in > this way for MAT_072r3 be applicable? > 3. ...Or is this a bug, which I should file as such? > > Alex Hay > Ticket#2017070610000015 ___________________________________________________________ Curve LCRATE is not rediscretized. Linear interpolation is used between data points. Ticket#2020021010000206 ----------------------------------- Eq.(1) and Eq.(4) are implemented when LCRATE=-1. [Refer http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/P-14-3_validateconcretelaws.pdf ] Youcai On 12/19/2016 04:09 PM, Todd Slavik wrote: > Youcai, > > Do you have documentation for the LCRATE= -1 feature? -------------------------------------------------------------------------------- Because your model is in microseconds, the abcscissa values of LCRATE should be input in 1/microseconds. For your model it would not be correct to use the LCRATE =-1 option, because the DIF equations in the paper implemented when using this option are in units of seconds. ah Ticket#2018020710000146 _______________________________________________________________________________________ The paper is here ... http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/kccm_paper.pdf We are finalizing the algorithm for impact penetration currently and it should be wrapped up shortly. Once we are done, we'll send you a beta version executable for your trial with an example input deck. Youcai 6/21/16 Ticket#2016062010000199 Two more questions on *MAT72_R3. I was at the User’s conference in Dearborn, and Dr. Wu presented using SPG with *MAT_72R3. Would it be possible for him to share an example input deck on this approach? Also, Dr. Wu mentioned a good overview paper on *MAT72_R3 that has a title beginning “Numerical modeling of concrete using a partially…” Wu & Crawford. Dr. Wu said he could share. Could we get it through you? _____________________________________________________ The parameters (automatic generated and regularization) for the model are developed based on element size between 1/4" and 4". Therefore, it is not suggested to use them out of this range. Thank you, Regards, Youcai This is just a simple question of mesh size. Did you have a valid mesh size range for the proper use of this material model, or can I use whatever size I like? Ticket#2016062010000199 6/20/16 _______________________________________________________-FYI, this report described a study pertaining to validating the capability afforded by the standard release of the Karagozian & Case (K&C) cementitious (or concrete) material model. In doing this, responses computed with the KCC-model for structural components comprised of either concrete or reinforced concrete were compared with results from tests. Comparisons of the responses computed for the structural components were shown for both quasi-static and blast loadings. Computed responses were also compared to data from standard material tests to demonstrate the basic capability afforded by the KCC-model. The analytic results shown were computed with the LS-DYNA code. The KCC-model is embedded in this code (i.e., Release III, Model MAT072R3 in LS-DYNA): Crawford, J.E., Wu, Y., Choi, H.-J., Magallanes, J.M., and Lan, S., "Use and Validation of the Release III K&C Concrete Material Model in LS-DYNA, TR-11-36.5, Karagozian and Case Structural Engineers, Burbank, California, July, 2012. http://www.kcse.com/assets/Uploads/TR-11-36-6-KCCM.pdf Best, Jim Kennedy 2/17/14 _____________________________________________________________________ unresolved EFG issue for mat_072r3: We implemented a way to use extra history variable to visualize the cracking in EFG fracture analysis. However, it is not compatible with the material type Matt is using and actually the crack never happens in his modeling, that's why the total energy keeps going up. I'll need some time to fix this bug. Please advise Matt to wait for my update. Yong Guo (in email to jday, 5/12/14, related to Ticket#2014050110000113 ) _____________________________________________________________________ We concluded that R7 is indeed the correct code implementation of MAT072_REL3. The R6 version is consistent with R7 IF all the inputs fields are input directly (i.e., the “direct input” option); however, there is a bug related to the “automatic” parameter generation option. In this R6 code and the “automatic” option, where most of the input card is typically set to zero, a line in the code that resets the b1 parameter to a default value was commented out; consequently, the R6 code was using a b1 value of 0 for all of “automatic” parameter option. This is the reason why I was so confused at the differences I was seeing between R6 and R7 for the problem I was handed to look at; here at K&C, we rarely use the “automatic” option (because I have a separate code that computes values for different types of concretes and concrete-like materials and input all the parameters directly). Let me know if this clears this issue up. Lastly, I still think there are some peculiarities between the Windows and Linux versions for R7, but I haven’t had time to put this in a format for you. I’ll see if I can reproduce some of those peculiarities and if I see them again I will send them over. Joe Magallanes@kcse.com 11/22/13 __________________________________________________ bugzilla 8972 describes bug affecting R60 and R61 (prior to 9/26/13). ____________________________________________________ RE: erosion There is no erosion criterion in the material model. Can use *mat_add_erosion. __________________________________________________________________________________ Bug #8512, making *mat_072r3 unstable when *damping_part_stiffness is applied, is fixed in v81304dev, R70.81305 on 5/2/13 (LL). __________________________________________________________________________ The sample curve tabulated in the User's Manual has strain rate units of 1/millisecond whereas your curve's abscissa should be in units of 1/second. Using 971 Dev, the messag (or mes0000) file will include a full set of material input parameters, generated internally based on the unconfined compressive strength provided by -A0. If NOUT=2, the "plastic strain" in the output actual represents the scaled damage measure (per Table 72.1 in the latest User's Manual). This damage is 1.0 when lambda = (lambda)m, signaling arrival at the maxium failure surface. As lambda increases from that point, the failure surface transitions between the maximum failure surface and the residual failure surface. Damage=2.0 signals arrival at the residual failure surface. The latest User's Manuals are always available at www.lstc.com/download/manuals . ____________________________________________________ we did try to let NPTS be greater than 13 to help regularization, but it is far away from mature, so we don't want to release it and let public users to try it now (that's why we didn't say anything about it in the Users Manual). So, my answer to your question is: NPTS<=13. Although the Users Manual says it must be 13, the code actually allows NPTS<13. But when user uses automatic generation, it will always be 13. Youcai 6/6/12 __________________________________________________ RE: output of parameters in convenient form to messag when automatic parameter generation is used. This was eariler disabled because of the unclear warning $ >>> Users need to change/check: MatID & RO & Rsize & LocWidth for units <<<" (Leslie incorp. below in v73017dev) Leslie: Please use this code [attached to email]. Note that parameter “ro” is added to the argument of subroutines “prmt72” and “prmt72r3”. Therefore, you need to add “ro” to the call statement “call prmt72(…)” in subroutine “printm”. With these changes, the output “messag” file is attached for the corresponding input “mat72r3.g-mm-ms.k”. By doing this, users can copy the keyword part of “*MAT_DAMAGE_CONCRETE_REL3” and “*EOS_TABULATED_COMPACTION” and make their own input easily. Now, RO, RSIZE, and UCF are the ones defined exactly by users in the automatic generation version, which is required! However, the MATID and EOS ID are purposely set to 72. The reason is, users have to change the *PART card when direct input is used (EOS ID must be input). Users are forced to change the MATID and EOS ID on both *PART and *MAT cards so that they are consistent and this CANNOT be done without any manual operation. Nevertheless, MATID and EOSID are just some arbitrary unique numbers that have nothing to do with the material properties. Youcai KCSE 3/28/12 ___________________________________________________________________ In my previous work, I did quite a bit of work with seismic loads, so I do appreciate the need and difficulty of the seismic problem. We've also discussed the concrete model with Bureau of Reclamation for some time now (in fact, I think we gave them a copy of the source code for an older version some time ago, but I am not sure). Most recently, Lawrence Livermore National Laboratories had an interest in seismic as well, but their interest had a slightly different twist. To answer your last questions: (1) "Yes, there is compression strength after tensile failure with confinement, even higher than the unconfined peak compression. Is this because the damage parameter does not go to 2 even though the tension stress is zero? The confined monotonic compression peak is almost 6000 psi (same confining pressure)." - The reason for this is that fractured concrete has a residual friction when placed under confinement, much like a sand or other cohesionless geomaterial will. This is encapsulated in the model with one of the three failure surfaces. When you are damaged closer to "2", the model interpolates toward the third "residual" strength failure surface; the higher the confinement, the higher the residual shear strength, which is consistent with data. (2) "One thing that seems odd is that the slope to failure in the softening range of compression is abrupt, almost vertical, but that of the tension is flatter. This holds true for both unconfined and confined. It seems it would be the other way around, unless I'm missing something. Any comments on that?" -I'm not sure I see what you mean. If you mean that the there are differences in the post-failure response in compression versus tension, this is just a function of several parameters that a user can vary if your data tells you otherwise. For blast, these "default" values work remarkably well, but you can change them with some experience using the model (see next question). (3) Is there any way to tweak the stress strain relationship to match test samples by plugging in some of the parameters rather than using the defaults? -Good question. Short answer is yes. The long answer is that I have developed a scheme consisting of a little art plus science to do this which is difficult to explain in an email. I am attaching a recent paper I put together that touches on this subject. See the section "Parameter Estimation Methodology". (see http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/Magallanes_et_al_2010b.pdf ) There are several avenues to take to attempt using the LS-DYNA concrete models for seismic applications, but I would definitely recommend V&V (verification and validation), since this is really an area that has not been explored with fully 3D continuum simulations. I can send you a technical report we put together that has a few example V&V seismic problems that we did several years ago if your interested. Bottom line is that the blast/impact concrete models including MAT072R3 is a very good option for this but there may be inevitable improvements needed to work your problem correctly. I'd be happy to discuss this, maybe even put some other people together in the Government who would be interested in this, since it does seem like an important application to cover. I'm traveling for the rest of the week (starting tomorrow), but am in my office if you would like to set up a time to discuss (818-240-1919). Joe Magallanes (in email to ggauthie@water.ca.gov) 11/29/11 Based on test data I have seen, the following occurs during stress reversals (again, limiting to unconfined cases, i.e., uniaxial stress): (1) Compression into the post-failure softening regime, then reversal in tension. After being heavily damaged in compression, there is very little tensile capacity. Test samples are faulted (at some inclined angle) if not heavily micro-cracked. (2) Tension into the post-failure softening regime, then compression reversal. The tensile failure will generate a crack plane perpendicular the the applied loading direction. Upon reversal, and after closure of that crack, there would be some resistance to compression, albeit at some reduction from its pristine capacity. MAT072R3 handles these two cases as follows: (1) Softening occurs when damage is between 1.0 to 2.0 (1.0 designates the maximum strength, while 2.0 is the maximum damage, as indicated by Jim, which softens the material to the residual failure surface). Since R3 uses one damage internal variable, tensile reversal stresses will be less than the pristine tensile strength. If the element is damaged up to 2.0 in compression, then the tensile strength upon reversal with be effectively zero. Although not perfect, this is consistent with test data. (2) When completely softened in tension (2.0), the compression stress will similarly be zero, effectively. I think Gary's point that this is unrealistic is well-taken, but this will only be true in the unconfined case (uniaxial stress). If you have some confinement (for example due to steel reinforcement or from the inertia of surrounding concrete), you will see that MAT072R3 will indeed have some compression resistance that is less than the maximum strength capacity. So again, not perfect, but consistent with data. This all being said, these issues are not unique to MAT072R3. I know at least two of the other concrete models in LS-DYNA would yield similar results. Most of those models were originally developed for blast/impact applications, where stress-reversals were not the primary interest. I don't know of much data that is available from which to calibrate reversal effects (I'd be happy to look at it if Gary and all have some). I also don't know of very many 3D continuum plasticity models that have been specifically developed/validated for seismic applications (would this be Gary's primary interest?), although our new version may better handle that (MAT072R4). I hoping to get that over to Jim and LSTC soon. Joe Magallanes 11/29/11 _______________________________________________________________________________ From correspondence with Len, 11/2010: 2. Perhaps that line in the code: ywhrt(i) = max(ywhr(i),ywhrt(i)) covers the case where the user inputs the DIF values in the wrong order, e.g. the DIFs for the negative entries (tension) are smaller than the DIFs for the positive entries (compression). That is your Define_Curve 99 case 3. The response is linear elastic if the initial yield has not been reached AND the mean stress is below the transition to the void collapse pressure, i.e. the linear elastic bulk modulus is operative. 4. Youcai Wu of K&C just mentioned Releases 4 in response to a question I asked at the meeting. Len -----Original Message----- Sent: Saturday, November 06, 2010 9:28 AM Subject: Re: Mat_072R3 with rate effects; Release 4 of K&C model 2. Good point about my test curves 8 and 9. In the attached model, I reconstituted curves 8 and 9 as curves 88 and 99 wherein the enhancement factor is 1.0 at zero strain rate. Using curve 99, I still find that for tension, peak tensile stress/nominal (unenhanced) tensile strength = 7.6/3.8 = 2, with the conclusion being that tensile strength enhancement = max [tensile rate enhancement from curve,compressive rate enhancement from curve] = max (1.5, 2.0] = 2.0 See http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/concrete/m72r3.rate_effects.k The source code for 72r3 appears to confirm it ... ... 3. Is the response of the material EVER linear, even in the low tensile strain and in the low compressive strain regimes? 4. Are there any publications that speak of the enhancements of Release 4? jd > > > > I want to understand your reply. > > > > 1. Your conclusion is that negative strain rate values in LCRATE > > correspond to tensile states, e.g. when the mean stress is negative. I agree with this. > > > > 2. I did not run your nice example, but I do not understand the caveat > > you > > mention: > > > > "There appears to be one caveat, i.e., tensile strength enhancement = > > max [tensile rate enhancement from curve, compressive rate enhancement > > from curve]" > > > > The only non-magnitude difference between LCRATE 8 & 9 is in the > > former the zero rate value is the same as the compressive value, and > > in the latter the zero rate value is the same as the tensile DIF. > > > > So why doesn't LCRATE 8 & 9 provide the same caveat? > > > > I also suggest you do not use anything other than UNITY for the > > zero-rate value in any LCRATE - this is not physical and I am unsure > > if the algorithm implementation depends on the unity at zero rate > > assumption; programmers do 'odd' things :) > > > > > > 3.If a user wants to adjust the elastic modulus, they will need to use > > the full input version of MAT072R3. > > > > > > Finally, last week I attended a session at the recent Shock & > > Vibration symposium where one of the K&C guys admitted they now have > > Release 4, but have not provided this releases to LSTC. ls _____________________________________________________________________ Yocai from Karagozian and Case reported seeing bad behavior of mat_072r3 when using solid ELFORM 2 and also when doing implicit analysis. He will contact John (6/27/08). I found a mat_072r3 example with solid elform 2 in our QA suite. Even in this QA problem involving penetration of mat_072r3 material, the elform 2 response is dubious as compared to the elform 1 response. On the basis of what I've seen in the test cases, I would say the prudent recommendation is not to use ELFORM 2 for mat_072r3. Alyotech also reported bad behavior of ELFORM 2 in reinforced concrete beam test case. _____________________________________________________________________ The information echoed to the 'messag' file includes the following: $ >>> Users need to change/check: MatID & RO & Rsize & LocWidth for units This warning was to indicate the values were hardwired, as these values were not readily available in the subroutine that wrote the 'messag' file information. Perhaps I should have been more explicit when writing this warning, or left the entries blank. --len _____________________________________________________________________ From emails 9/22/06 thru 9/25/06 (home machine) Thanks Javier. [Your comments are worth much more than 2-cents! :)] #1 - I mis-read Jim Day's plot, the scaled damage parameter did NOT exceed TWO. So all is OK with this part of Mat072R3. #2 - Jim - are you aware of LSTC receiving updates from K&C? Thanks again Javier, --len -----Original Message----- From: malvarl [mailto:malvarl@adelphia.net] Sent: Sunday, September 24, 2006 9:34 PM To: Len@Schwer.net; 'Jim Day' Cc: torodd@lstc.com; 'Jensen'; 'Mediavilla Varas, J. (Jesus)' Subject: RE: Nonlocal and mat72_r3 Hi Len My 2 cents: #1 - Since the scaled damage parameter = 2L/(L+Lm) where L = lambda, and Lm = lambda at maximum failure surface, epx1 would tend to 2, but should not really reach it, nor exceed it (it is 1 if L = Lm). #2 - In quasi-static runs, the failure using Mat72R3 will not diffuse, but it should expand the same amount of fracture energy. Unfortunately, there is a bug in the current LS-DYNA version which makes this happen only if the mesh has uniform elements - this has been corrected and will be passed on to LS-DYNA. Thanks Javier -----Original Message----- Sent: Saturday, September 23, 2006 12:31 PM Subject: RE: Nonlocal and mat72_r3 I spent sometime looking at this problem and have two observations. #1 - I think the problem as posed by Jesus of a fixed-end rod under step tensile loading is not suitable for examining the effect of *Mat_NonLocal. The fixed-end causes the tensile wave to double and this fails the element closest to the fixed end. I doubt refining the mesh will change this results, as this is what the physics also predicts. I guess it was hoped that *Mat_NonLocal would "smear out" this end failure. Apparently it cannot in this case, which in my assessment is the right thing; but as always I could be wrong about this and everything else. BTW - the scaled damage parameter, epx1 in this case, should range between ZERO (no damage) to UNITY at the failure surface and then TWO when the residual failure surface is reached. Why values greater than TWO are reported in this problem is unknown; perhaps Javier can comment on this? #2 - To see if *Mat_NonLocal is working with Mat072R3, I modified Jesus' problem to be quasi-static with a prescribed displacement rather than a stress end load. [There is still perhaps a bit too much dynamics in this simulation, but I get paid by the hour so I do not run freebie jobs for too long :)] I also introduced a 'random' mesh scale along the length of the rod. The function of *Mat_NonLocal is to prevent strain from accumulating in the small (shortest) element. So if the mesh is uniform, the strain should not accumulate in any one place and hence such a uniform mesh is not a good test of *Mat_NonLocal. I ran the above described (and attached) model twice: Case 1 - omitting *Mat_NonLocal Case 2 - with *Mat_NonLocal setting L=100 [nominal cube root of element volume is about 36=(20x50*50)^(-1/3)] When *Mat_NonLocal is omitted, Case 1, the failure (strain) localizes in Element #49, which is the second shortest element length in the rod; the relative element lengths can be observed in the d3hsp file by looking at the list of smallest time steps. For Case 2, with *Mat_NonLocal, the failure is diffused over several elements; mostly in the vicinity of Element #49. It might be worthwhile to run this implicit/static to see what (really) happens? So I think *Mat_NonLocal is working with Mat072R3. The troubling part to me is omitting *Mat_NonLocal SHOULD also diffuse the failure as Javier has a built-in localization limiter in the parameter LocWidth(=100 in this case). Perhaps Javier can comment on this? ls -----Original Message----- Sent: Friday, September 22, 2006 12:04 PM Subject: Re: Nonlocal and mat72_r3 Just looking at the fine mesh problem, *mat_nonlocal definitely affects epx1 ("effective plastic strain" which is supposedly the scaled damage function) of some elements but such that epx1 is not monotonically increasing (see attached jpeg). Make any sense to you? Also, should epx1 be in the range of 0 <= epx1 <= 1.0? jd >> I did the 1D simulations as ls suggested. Unfortunately I do have >> mesh dependent results. See attached figures. >> >> After reflexion on the fixed end, strain localizes in one element. >> >> >> I have tried as nonlocal variables, NL=1 and also NL=7, with the >> damage scaled variable NOUT set to 2. >> I'm sending you the indeck files corresponding to three different >> meshes. Perhaps you can take a look. >> >> I have switched off the strain rate hardening, because this might (and >> it does) regularize the problem.