Tool (software) for user defined material model subrountine

- September 23, 2019 at 7:36 pm
  
  zhonghu
  Subscriber
  
  Hello,
  
  I am planning to write a user defined material model subroutine USERMAT compiling with ANSYS, I am wondering if gfortran 4.8.5 is a good one to use for writing and compiling, and currently the what version of fortran ANSYS used? fortran 95/2003/2008? and where is the link to read the interface of the USERMAT? Anything else I need to prepare before starting writing the code?
  
  Thanks
- October 16, 2019 at 2:23 pm
  
  peteroznewman
  Subscriber
  
  I moved this Discussion to Structural from Embedded Software for better visibility.
- October 16, 2019 at 8:05 pm
  
  David Weed
  Ansys Employee
  
  Hi,
  
  Can you let me know which release of ANSYS you are using? We don't support gfortran, but rather Intel Fortran compilers for both Windows and Linux platforms.
- October 21, 2019 at 4:26 pm
  
  zhonghu
  Subscriber
  
  Hello David,
  
  Thanks for your response and info. Right now I am using the latest version ANSYS 19.3R research license and planing to write the USERMAT in unix with codeblocks GNU GCC Compiler or GNU Fortran Compiler. I am not sure if it is ok. Also I am wondering if you can advice me the interface format of the USERMAT.
  
  Many thanks,
  
  Zhong
- October 21, 2019 at 5:31 pm
  
  zhonghu
  Subscriber
  
  sorry, I should be working on Linux platform.
- October 25, 2019 at 11:22 pm
  
  David Weed
  Ansys Employee
  
  Hi Zhong,
  
  You can find the compiler requirements for R19.3 on the Linux Platform here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v193/installation/installation_set_cbn_sqj_r5.html?q=compiler
  
  Intel 17.0.4 (FORTRAN, C, C++) and GCC 6.3.0 (for user programmable features)
  
  Please note that GCC 6.3.0 is only available through ANSYS, Inc. Customers are required to go through the Customer Portal to download the compiler there. You may have to discuss doing procuring this with your account manager. Also, for the Intel Fortran compiler, you need an Intel account and your institution would have to purchase the compiler. Please only use the specific software versions listed in the link above. We can't ensure that routines will successfully compile or produce reliable results outside of those versions.
- October 29, 2019 at 11:00 pm
  
  zhonghu
  Subscriber
  
  Hi David,
  
  Thanks for your info. Now I have some other questions for you:
  
  (1) What files I need to load in my account on the server machine before I can compile my usermat.f with ANSYS and does ANSYS can provide all these files (such as all MAPDL files);
  
  (2) Where I can find the current version of the example of usermat3d.f I can check out or compare with mine.
  
  Thanks,
- October 30, 2019 at 7:51 pm
  
  zhonghu
  Subscriber
  
  Hi David,
  
  Looks like I found the necessary ANSYS files under the ansys/customize/user folder. Now I left one more question is that can you send me or tell me where the usermat3d example, I need check with mine to see the compatibility to this ansys2019r3 version.
  
  Thanks.
- October 30, 2019 at 8:27 pm
  
  zhonghu
  Subscriber
  
  Hi David,
  
  Ok, I found it in the same folder, but it was generated in 1999, so I guess its format doesn't change. So I can test the compiler I have installed of the Intel.
  
  Thanks,
- October 31, 2019 at 4:31 pm
  
  David Weed
  Ansys Employee
  
  Hi Zhong,
  
  Yes, usermat3D is a subroutine within usermat.F itself. From what I've heard, these routines have changed very little, if at all, since their initial inception.
- October 31, 2019 at 5:42 pm
  
  zhonghu
  Subscriber
  
  Hi David,
  
  When I compile I need compile all the files in the folder, not just the files with .F?
  
  Thanks,
- November 1, 2019 at 10:37 pm
  
  David Weed
  Ansys Employee
  
  Hi Zhong,
  
  I would suggest reading the help which details the different compilation/linking methods: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v193/ans_prog/GxI4r398wfl.html. You can create a separate directory specifically for compiling your routines; it should contain the script for whichever compile method you've chosen (e.g., /UPF or shared library) and the routines of interest. You also mentioned using an unsupported compiler; this section may be relevant:
  
  ANSYS, Inc. recommends using the ANSUSERSHARED script as a template to try compilers that are not supported by ANSYS, Inc., such as the GNU compilers. To do so, edit the ANSUSERSHARED script, making changes to the appropriate platform logic. Note that if you do use compilers other than those listed in the ANSYS Installation and Configuration Guide specific to your operating system, you will need to debug (i.e., find missing libraries, unsatisfied externals, etc.) them yourself. ANSYS, Inc. does not provide assistance for customers using unsupported compilers or if the resulting objects are not compatible with the executable(s) as distributed.
- December 20, 2019 at 4:49 pm
  
  zhonghu
  Subscriber
  
  Hello David,
  
  Yes, I made the user customized system work.
  
  I did a test by using ANSYS BISO material and the USERMAT (ANSYS provided sample BISO), I found something different:
  
  (1) Test conditions: A cylindrical (Axi-symmetric) metallic volume with radius of 20 mm and height of 40 mm undergone a 4% tension;
  
  (2) Material data: Young's modulus E = 220.8 GPa, Poisson's ratio = 0.3, Yield strength = 1137.7 MPa, Strain Hardening slope H = 1466.0 MPa
  
  (3) Results extracted from the data: The tension displacement (Uy), tension force (Fy), average von Mises stress (S eqv, actually it is a uniform deformation, every element has the same value), average von Mises elastic strain (EPEL eqv, every element has the same value), and von Mises plastic strain (EPPL eqv, every element has the same value);
  
  (4) The same: Under the same load step, both ANSYS BISO and USERMAT provided the same Uy, Fy, von Mises stress, von Mises plastic strain;
  
  (5) Difference: However, at the beginning of tension, it is elastic deformation, so the Young's modulus should be the ratio of the von Mises stress to the von Mises elastic strain, the result from ANSYS BISO provided the right answer, compared to the Young's modulus input in the batch file, but the result from USERMAT is not right (smaller elastic strain, resulting in higher Young's modulus); also all the elastic strains during the tension from USERMAT are smaller than that from ANSYS BISO;
  
  Attached please find the APDL input batch file and the result files from ANSYS BISO and USERMAT;
  
  Can you take a look if there is anything wrong? Since I really care about the elastic strain and my project needs very accurate elastic strain modeling.
  
  By the way, I am wondering if ANSYS can share BKIN subroutine with me, since I am developing a subroutine with a very unique Bauschinger effect (not the 2 time yield stress 2Y by BKIN, but would be very helpful).
  
  Thanks and happy holidays,
  
  Zhong
  
  APDL batch file input
  
  ! This is a Tension-Compression testing using USERMAT BISO for A723-1130
  
  /FILNAM, Tension_USERMAT-ANSYS_BISO
  
  !/TITLE, This is a Tension-Compression testing using USERMAT BISO A723-1130 material input
  
  /UNITS,user !Length-mm, force-N, stress-MPa
  
  !Specimen dimensions
  
  r_=20 !width of specimen
  
  h_=40 !depth of specimen
  
  ! generate model
  
  /PREP7
  
  ET,1,PLANE183,0,,1, !2-D 8-node for specimen
  
  ! keyopt(1)=0, 8-node quadrilateral; keyopt(3)=1, axisymmetric
  
  !!ANSYS BISO input
  
  MP,EX,1,220.8122966e3 !Young's modulus and Poisson ratio for tension
  
  MP,PRXY,1,0.3 !Poisson's ratio
  
  TB,BISO,1,1
  
  TBTEMP,0
  
  TBDATA,1, 1137.708703, 1466.033865 ! Sigy0, H
  
  !!Usermat BISO input
  
  !TB,User,1,1,4 !User defined Bi-linear with four inputs
  
  !TBTEMP,0
  
  !TBDATA,1,220.8122966e3, 0.3, 1137.708703, 1466.033865 !E, Posn, Sigy0, H
  
  !TB,STATE,1,,16
  
  !Generate model for the specimen
  
  K,1,0,0
  
  K,2,r_,0
  
  K,3,r_,h_
  
  K,4,0,h_
  
  A,1,2,3,4
  
  LESIZE,1,,,20
  
  LESIZE,2,,,40
  
  LESIZE,3,,,20
  
  LESIZE,4,,,40
  
  TYPE,1
  
  MAT,1
  
  Amesh,1
  
  save
  
  finish
  
  /solution
  
  ANTYPE,trans,new
  
  nlgeom,on
  
  nropt,full,on
  
  !predict,off
  
  neqit,20
  
  ncnv,0
  
  solcontrol,on
  
  cnvtol,f,,0.01
  
  cnvtol,u,,0.01
  
  !AUTOTS,ON !!!!
  
  ! define displacement boundary conditions on the axisymmetric axis of the specimen
  
  NSEL,S,loc,x,0
  
  D,all,ux,0
  
  NSEL,all
  
  ! define displacement boundary conditions on the bottom of the specimen
  
  NSEL,s,loc,y,0 ! select nodes at the bottom
  
  D,all,uy,0
  
  NSEL,all
  
  !!!!!! apply 4% the tension displacement on the top surface of the specimen
  
  NSEL,s,loc,y,h_
  
  D,all,uy,0.04*h_
  
  NSEL,all
  
  TIME,1
  
  DELTIM,0.005,0.001,0.01
  
  OUTRES,all,-100
  
  KBC,0
  
  SOLVE
  
  save
  
  fini
  
  /post26
  
  STORE,NEW
  
  NSEL,S,LOC,y,h_
  
  *GET,NODETOT,NODE,,COUNT
  
  *GET,MINNODE,NODE,,NUM,MIN
  
  nsol,2,MinNode,u,y,DispY
  
  RFORCE,3,MinNode,F,Y
  
  *GET,SigEqv,NODE,MinNode,s,eqv
  
  NODENUM=MINNODE
  
  *do,i,1,NodeTot-1,1
  
  NodeNum=ndnext(NodeNum)
  
  rforce,4,NodeNum,f,y
  
  add,3,3,4,,Load,,,1,1
  
  *enddo
  
  add,3,3,,,Load,,,1
  
  add,2,2,,,Disp,,,1
  
  NSEL,all
  
  ESEL,all
  
  *GET,ELEMTOT,ELEM,,COUNT
  
  *do,i,1,ELEMTOT,1
  
  ESOL,6,i,,S,EQV,SEQV
  
  ADD,5,5,6,,SEQV,,,1,1
  
  ESOL,8,i,,EPEL,EQV,EEEQV
  
  ADD,7,7,8,,EEEQV,,,1,1
  
  ESOL,10,i,,EPPL,EQV,EPEQV
  
  ADD,9,9,10,,EPEQV,,,1,1
  
  *enddo
  
  add,2,2,,,Disp,,,1
  
  add,3,3,,,Load,,,1
  
  add,5,5,,,SEQV,,,1/ELEMTOT
  
  add,7,7,,,EEEQV,,,1/ELEMTOT
  
  add,9,9,,,EPEQV,,,1/ELEMTOT
  
  *dim,T_Data,array,100
  
  *dim,Dy_Data,array,100
  
  *dim,Fy_Data,array,100
  
  *dim,Si_Data,array,100
  
  *dim,Eli_Data,array,100
  
  *dim,Epi_Data,array,100
  
  vget,T_Data(1),1
  
  vget,Dy_Data(1),2
  
  vget,Fy_Data(1),3
  
  vget,Si_Data(1),5
  
  vget,Eli_Data(1),7
  
  vget,Epi_Data(1),9
  
  /xrange,0,0.04*h_
  
  /yrange,0,2000000
  
  /grid,1
  
  xvar,2
  
  plvar,3
  
  /output,Tension_ANSYS_BISO_Data,txt,,append
  
  !/output,Tension_USERMAT_BISO_Data,txt,,append
  
  *vwrite,T_Data(1),Dy_Data(1),Fy_Data(1),Si_Data(1),Eli_Data(1),Epi_Data(1)
  
  (6(F18.6,2x))
  
  /output
  
  fini
  
  Data from ANSYS BISO
  
  time Tension Uy (mm) Tension Fy (N) von Mises Seqv(MPa) Elastic strain eqv Plastic strain eqv
  
  0.010000 0.016000 110943.548964 88.307259 0.000400 0.000000
  
  0.027500 0.044000 304860.088252 242.760025 0.001099 0.000000
  
  0.037500 0.060000 415535.645173 330.970276 0.001499 0.000000
  
  0.047500 0.076000 526113.972334 419.145294 0.001898 0.000000
  
  0.057500 0.092000 636595.187567 507.285126 0.002297 0.000000
  
  0.067500 0.108000 746979.408514 595.389771 0.002696 0.000000
  
  0.077500 0.124000 857266.752633 683.459290 0.003095 0.000000
  
  0.087500 0.140000 967457.337195 771.493713 0.003494 0.000000
  
  0.097500 0.156000 1077551.279287 859.493042 0.003892 0.000000
  
  0.107500 0.172000 1187548.695808 947.457275 0.004291 0.000000
  
  0.117500 0.188000 1297449.703475 1035.386475 0.004689 0.000000
  
  0.127500 0.204000 1407254.418817 1123.280762 0.005087 0.000000
  
  0.137500 0.220000 1425411.889183 1138.196289 0.005155 0.000330
  
  0.147500 0.236000 1425576.512573 1138.779297 0.005157 0.000725
  
  0.157500 0.252000 1425740.715944 1139.362183 0.005160 0.001120
  
  0.167500 0.268000 1425904.500026 1139.944824 0.005163 0.001515
  
  0.177500 0.284000 1426067.865545 1140.527222 0.005165 0.001910
  
  0.187500 0.300000 1426230.813230 1141.109375 0.005168 0.002304
  
  0.197500 0.316000 1426393.343804 1141.691284 0.005170 0.002699
  
  0.207500 0.332000 1426555.457993 1142.272949 0.005173 0.003093
  
  .........
  
  Data from USERMAT
  
  time Tension Uy (mm) Tension Fy (N) von Mises Seqv(MPa) Elastic strain eqv Plastic strain eqv
  
  0.010000 0.016000 110943.548964 88.307259 0.000347 0.000000
  
  0.027500 0.044000 304860.088252 242.760025 0.000953 0.000000
  
  0.037500 0.060000 415535.645173 330.970276 0.001299 0.000000
  
  0.047500 0.076000 526113.972334 419.145294 0.001645 0.000000
  
  0.057500 0.092000 636595.187567 507.285126 0.001991 0.000000
  
  0.067500 0.108000 746979.408514 595.389771 0.002337 0.000000
  
  0.077500 0.124000 857266.752633 683.459290 0.002683 0.000000
  
  0.087500 0.140000 967457.337195 771.493713 0.003028 0.000000
  
  0.097500 0.156000 1077551.279287 859.493042 0.003373 0.000000
  
  0.107500 0.172000 1187548.695808 947.457275 0.003719 0.000000
  
  0.117500 0.188000 1297449.703475 1035.386475 0.004064 0.000000
  
  0.127500 0.204000 1407254.418817 1123.280762 0.004409 0.000000
  
  0.137500 0.220000 1425411.889183 1138.196289 0.004467 0.000330
  
  0.147500 0.236000 1425576.512573 1138.779297 0.004470 0.000725
  
  0.157500 0.252000 1425740.715944 1139.362183 0.004472 0.001120
  
  0.167500 0.268000 1425904.500026 1139.944824 0.004474 0.001515
  
  0.177500 0.284000 1426067.865545 1140.527222 0.004476 0.001910
  
  0.187500 0.300000 1426230.813230 1141.109375 0.004479 0.002304
  
  0.197500 0.316000 1426393.343804 1141.691284 0.004481 0.002699
  
  0.207500 0.332000 1426555.457993 1142.272949 0.004483 0.003093
  
  ...........
- March 11, 2020 at 3:34 pm
  
  AntiNeutrino03
  Subscriber
  
  Can the community edition of the Fortran Compilers and Visual studio be used for UDFs?
  
  Also, do the later versions of the compilers work?