Programming

FEAP is designed to allow users to modify the code for their owm purposes. If at all possible, users should always use the user hooks provided in the user directory. These allow users to make custom elements, material models, new FEAP commands, et cetera. The programmers manual provides an introduction to programming in FEAP.

To use the user hooks, it is recommended to make a copy of the relevant stub file in a separate project directory. Then add the full path name to this edited copy to main/makefile on the OBJECTS line so that it will be built into FEAP the next time you compile it. If you are using windows, add the copy to your executable project. Even though there is a version of the stub file in your FEAP archive file, the compiler should use your edited copy instead of the one in the archive.

It is also recommended that you obtain a good Fortran reference book, e.g. Modern Fortran Explained by Metcalf, Reid, and Cohen.

Programmers Manual

The programmers manual can be found on the FEAP project site http://projects.ce.berkeley.edu/feap.

User Elements

AceGen and Mathematica

A template has been developed for generating user elements in an automated manner using AceGen and Mathematica. The Mathematica files, the generated user elements, examples, and benchmark examples can be found on the FEAP-AceGen GitHub repository. Detailed documentation about the template can be found in the SEMM report (UCB/SEMM-20211/01).

User Materials

The method to implement a user material model in FEAP has been described in Section 4.2 of FEAP Programmer Manual. Here we would like to clarify a few things in the user material model with history variables.

The time-dependent history variables

The time-dependent variables are meant to be used for quantities that change in "TIME". That is if you have a solution that advances from time $t_{n}$ to $t_{n+1}$ the history variables for $t_{n}$ are stored in hr(nh1) and those for $t_{n+1}$ are stored in hr(nh2). These can be state variables in incremental stress-strain relations. In your solution algorithm, you must use the solution commands TIME and DT. The structure of your user material model should look like this:

1. In your umati*.f routine, set n1 equals the number of history variabales per Gauss point.

2. In your umodelf.f or umatl*.f subroutine, read the history variables from the previous globally converged time step $t_{n}$ from hn(*)

3. Compute new values of history variables

4. Write your newly computed history values to h1(*) for next time step $t_{n+1}$. Do not write to hn(*)!

After that, FEAP will carry out a global Newton iteration.  If the global Newton iteration is not converged, then the values you wrote to h1(*) will be discarded and your routine will be called again. You will repeat again from step 2 until it is converged. Then, the values in h1(*) will be copied over into hn(*) for use in the next time step when you execute the next TIME command.

The time-independent history variables

If the history variable does not depend in time then we consider them to be independent of "TIME", so you could use the time-independent history variables as it only stores one copy of each value instead of two in the previous case. This type of history variable is more like a status variable depending on deformation. Here is the procedure to implement such kind of history variables,

1. In your umati*.f routine, set n3 equals the number of history variables per element.

2. In your umodelf.f or umatl*.f subroutine, read the history variables from the previous globally converged time step $t_{n}$ from hr(nh3+i) where i runs from 0 to the number of history variables (per gauss point) minus one and nh3 points to the location of first history variable for the current Gauss point.

3. Compute new values of history variables.

4. Update history variables in hr(*) with the newly computed values if needed.

Initialization of history variables in element or materials routines

The history variables are initialized to zero by default. But if you want to initialize any of the history variables to non-zero values you can do this when ISW .eq. 14. For example, if we have m history variables per gauss point, then you can initialize the time-dependent history variables to 1.0d0 in your umodelf.f or umatl*.f subroutine as follows,

c... INITIALIZE HISTORY VARIABLES
        IF (ISW .EQ. 14) THEN
            do i = 1, m 
                hn(i) = 1.0d0
                h1(i) = 1.0d0  
            end do 
        END IF

For time-independent history variables,

c... INITIALIZE HISTORY VARIABLES
        IF (ISW .EQ. 14) THEN
            do i = 0, (m - 1)
                hr(nh3 + i ) = 1.0d0
            end do 
        END IF

This segment of code will be executed for each Gauss point of each element.

(Note that this page is under development)

Calling MATLAB functions from FEAP

MATLAB functions can be called from FEAP if you have installed the MATLAB Engine (toolbox) when you set up MATLAB on your computer. The basic steps to getting this work are gone over below for a specific use case where I would like to use a MATLAB (*.m) file to compute a material model response for a user material.

The basics steps are as follows. (1) Have MATLAB and the MATLAB Engine installed. (2) Create a user macro that will start the MATLAB engine. This permits communication between the MATLAB data space and FEAP's data space using Unix sockets. (3) Set up your user material routine to send FEAP data to MATLAB to compute the material response and to receive is back from MATLAB. (4) Edit the makefile to allow for the compilation of subroutines with special MATLAB function calls as well as linking of the main program with the MATLAB Engine.

Setup the MATLAB Engine

The code to start up the MATLAB Engine will be placed in a user macro. To initialize the MATLAB Engine we just need to call this macro command once at the start of a FEAP run. For concreteness we use umacr6. It is important to save the file using a .F extender instead of .f, so that the compiler will run the preprocessor on it before compiling; this is all tested on a Mac which should be the same as Linux too. In the routine there are two user customizable strings: (a) The path to the matlab executable, '/Applications/MATLAB_2019a.app/bin/matlab' in my case, and the path to where my MATLAB *.m files are located, '/Users/sg/Feap/ver86/main' in my case. To use the macro, just type MLENgine at the macro prompt.

!$Id:$
      subroutine umacr6(lct,ctl)

!      * * F E A P * * A Finite Element Analysis Program

!....  Copyright (c) 1984-2019: Regents of the University of California
!                               All rights reserved

!-----[--.----+----.----+----.-----------------------------------------]
!     Modification log                                Date (dd/mm/year)
!       Original version                                    01/11/2006
!       1. Remove 'prt' from argument list                  09/07/2009
!       2. Add 'uhelpfl' comment option                     19/10/2017
!       3. Add 'help' comment option - replaces 'uhelpfl'   07/01/2019
!       4. Create the ML Engine init macro                  10/16/2019
!-----[--.----+----.----+----.-----------------------------------------]
!      Purpose:  Initialize the MATLAB Engine

!      Inputs:
!         lct       - Command character parameters
!         ctl(3)    - Command numerical parameters

!      Outputs:
!         N.B.  Users are responsible for command actions.  See
!               programmers manual for example.
!-----[--.----+----.----+----.-----------------------------------------]
      implicit  none

#     include "fintrf.h"
#     include "mleng.h"

      include  'iofile.h'
      include  'umac1.h'

      mwPointer engOpen
      integer :: status, engEvalString

      character (len=15) :: lct

      logical       :: pcomp
      real (kind=8) :: ctl(3)

      save

!     Set command word

      if(pcomp(uct,'mac6',4)) then      ! Usual    form
        uct = 'mlen'                    ! Specify 'name'

      elseif(pcomp(lct,'help',4)) then  ! Write help information

        write(*,*) 'COMMAND: MLENgine inits Matlab Engine'

      elseif(urest.eq.1) then           ! Read  restart data

      elseif(urest.eq.2) then           ! Write restart data

      else                              ! Perform user operation

        ep = engOpen('/Applications/MATLAB_R2019a.app/bin/matlab')

        if (ep.eq.0) then
          write(*,*) 'WARNING: Matlab engine failed to initialize'
          call plstop
        endif
        status = engEvalString(ep,'addpath /Users/sg/Feap/ver86/main')
        if (status.ne.0) write(*,*) 'WARNING: Matlab path not set'


      endif

      end subroutine umacr6

Note that this macro also includes two *.h files

#     include "fintrf.h"
#     include "mleng.h"

The first is a MATLAB file and is located in the MATLAB application directory. The second, I have placed in my FEAP main directory. It contains the pointer to the MATLAB Engine object that is returned by the endOpen() function call. It contents are

      mwPointer      ep
      common /mleng/ ep

User material

First I need a user material input routine. This is standard, except I am going to be lazy and not read in any material properties (they will be hard wired in the code). I will use umati6.f and give it the user name MLMAterial.

!$Id:$
      subroutine umati6(vtype,vv, d, ud, n1,n3)

!      * * F E A P * * A Finite Element Analysis Program

!....  Copyright (c) 1984-2019: Regents of the University of California
!                               All rights reserved

!-----[--.----+----.----+----.-----------------------------------------]
!     Modification log                                Date (dd/mm/year)
!       Original version                                    01/11/2006
!-----[--.----+----.----+----.-----------------------------------------]
!      Purpose: User input for material model 6

!      Inputs:
!         vtype  - Name of material model
!         vv(5)  - Command line real data
!         d(*)   - Program material parameter data

!      Outputs:
!         ud(*)  - Material parameter data for model
!         n1     - Number of history items/point (time   dependent)
!         n3     - Number of history items/point (time independent)
!-----[--.----+----.----+----.-----------------------------------------]
      implicit  none

      character (len=15) :: vtype

      logical       :: pcomp
      integer       :: n1,n3
      real (kind=8) :: vv(5),d(*),ud(*)

!     Set command name

      if(pcomp(vtype,'mat6',4)) then     ! Default  form DO NOT CHANGE
        vtype = 'mlma'                   ! Specify 'name'

!     Input user data and save in ud(*) array

      else                              ! Perform input for user data

      endif

      end subroutine umati6

The stress-strain routine

The stress strain routine will be linear elastic where the material properties will be hard wired into the MATLAB routine that computes the response based on the strain. This is done in a MATLAB umatl6.m file which I place in my FEAP main directory (since that is where I told MATLAB to find such files). The files looks like:

function [sig,dd] = umatl6(eps)
% Compute the stress and moduli
% Linear isotropic elastic material with hardwired
% Elastic properties

% 6x6 symmetric identity
Isym      = eye(6,6);
Isym(4,4) = 0.5;
Isym(5,5) = 0.5;
Isym(6,6) = 0.5;

% 6x6 id outer-product id
ooo          = zeros(6,6);
ooo(1:3,1:3) = 1.0;

% Lame parameters
mu    = 10;
lambd = 10;

% Elasticity moduli 6x6
dd = 2*mu*Isym + lambd*ooo;

% Stress 6x1
sig = dd*eps;

end

It expects a 6x1 strain vector and returns a 6x1 stress vector and a 6x6 modulus matrix. My FEAP user material subroutine will call this MATLAB function with the strain and receive back the stress and modulus. Since I am using user material 6, I place my FEAP code in umatl6.F; note the .F extender so that the preprocessor does its job correctly.

!$Id:$
      subroutine umatl6(eps,theta,td,d,ud,hn,h1,nh,ii,istrt, sig,dd,isw)
!     subroutine umatl6( f ,detf ,td,d,ud,hn,h1,nh,ii,istrt, sig,dd,isw)

!      * * F E A P * * A Finite Element Analysis Program

!....  Copyright (c) 1984-2019: Regents of the University of California
!                               All rights reserved

!-----[--.----+----.----+----.-----------------------------------------]
!     Modification log                                Date (dd/mm/year)
!       Original version                                    01/11/2006
!-----[--.----+----.----+----.-----------------------------------------]
!     Purpose: User Constitutive Model 6

!     Input:
!          eps(*)  -  Current strains at point      (small deformation)
!                  -  Deformation gradient at point (finite deformation)
!          theta   -  Trace of strain at point
!                  -  Determinant of deformation gradient
!          td      -  Temperature change
!          d(*)    -  Program material parameters (ndd)
!          ud(*)   -  User material parameters (nud)
!          hn(nh)  -  History terms at point: t_n
!          h1(nh)  -  History terms at point: t_n+1
!          nh      -  Number of history terms
!          ii      -  Current point number
!          istrt   -  Start state: 0 = elastic; 1 = last solution
!          isw     -  Solution option from element

!     Output:
!          sig(*)  -  Stresses at point.
!                     N.B. 1-d models use only sig(1)
!          dd(6,*) -  Current material tangent moduli
!                     N.B. 1-d models use only dd(1,1) and dd(2,1)
!-----[--.----+----.----+----.-----------------------------------------]
      implicit none

#     include "fintrf.h"
#     include "mleng.h"

      mwPointer mxCreateDoubleMatrix, engGetVariable
      mwPointer ml_eps, ml_sig, ml_dd
      mwSize    N, M
#if MX_HAS_INTERLEAVED_COMPLEX
      mwPointer mxGetDoubles
#else
      mwPointer mxGetPr
#endif

      integer       :: status, engPutVariable, engEvalString

      integer       :: nh,istrt,isw, ii
      real (kind=8) :: td
      real (kind=8) :: eps(*),theta(*),d(*),ud(*),hn(nh),h1(nh)
      real (kind=8) :: sig(*),dd(6,*)

      if (isw.eq.3 .or. isw.eq.6 .or. isw.eq.4 .or. isw.eq.8) then
!     Compute and output stress (sig) and (moduli)

      ! Initialize Matlab data space (should be done just once
      ! instead of each time with a destroy).  Important use
      ! mwSize typed variables for all sizes
      N = 6
      M = 1
      ml_eps = mxCreateDoubleMatrix(N,M,0) 

      ! Copy strains to Matlab data space
#if MX_HAS_INTERLEAVED_COMPLEX
      call mxCopyReal8ToPtr(eps, mxGetDoubles(ml_eps), N)
#else
      call mxCopyReal8ToPtr(eps, mxGetPr(ml_eps), N)
#endif      
   
      ! Place data in the MATLAB workspace (should pass along d, ud, hn, h1)
      status = engPutVariable(ep, 'eps', ml_eps)
      if (status.ne.0) then
        write(*,*) 'WARNING: sending strain to Matlab failed'
      endif

      ! Call the Matlab stress-strain function
      status = engEvalString(ep,'[sig,dd] = umatl6(eps);')
      if (status.ne.0) then
        write(*,*) 'WARNING: mymat.m eval failed'
      endif

      ! Get the stress and tangent from Matlab
      ml_sig = engGetVariable(ep, 'sig')
      ml_dd  = engGetVariable(ep, 'dd')
#if MX_HAS_INTERLEAVED_COMPLEX
      call mxCopyPtrToReal8(mxGetDoubles(ml_sig), sig,   N)
      call mxCopyPtrToReal8(mxGetDoubles(ml_dd ), dd , N*N)
#else
      call mxCopyPtrToReal8(mxGetPr(ml_sig), sig,   N)
      call mxCopyPtrToReal8(mxGetPr(ml_dd ), dd , N*N)
#endif

      call mxDestroyArray(ml_eps)
      call mxDestroyArray(ml_sig)
      call mxDestroyArray(ml_dd )

      endif

      end subroutine umatl6

There is a lot to be explained here, best is to review the MATLAB Engine documentation, but here are a few main points. (1) For every variable that you will send to MATLAB you need to create a pointer to its MATLAB version. This is done with the function mxCreateDoubleMatrix() for double precision arrays. It takes 3 arguments, number of rows, number of columns, and flag for if it is complex or not. This command creates the pointer. The MATLAB pointer is hooked to your FEAP Fortran array using mxCopyReal8ToPtr() (the syntax of which depends on your MATLAB version, which the preprocessor figures out). (2) To send data from Fortran arrays to MATLAB arrays one uses the engPutVariable() function. (3) To execute MATLAB commands in the MATLAB data space one uses the engEvalString() function. In our case we evaluate the MATLAB function umatl6() which we wrote. The return values end up in sig and dd in the MATLAB data space. (3) To retrieve the values, we first set up a pointers to these MATLAB arrays using the engGetVariable() function. We then copy the data from these pointers to our FEAP Fortran arrays using the mxCopyPtrToReal8() function. (4) Lastly, I destroy all the pointers with mxDestroyArray().

Note there is a bit of waste here. I should create the pointers only once and then destroy them only once where I terminate FEAP but that requires being more sophisticated and makes it harder to understand the basic steps.

Setting the makefiles

To get this all to compile, you need to edit the makefile in FEAP's main folder. It needs to be able to find the MATLAB system include files and the location of the MATLAB libraries. What you see below, is what I needed on my Mac.

include ../makefile.in

MLROOT = /Applications/MATLAB_R2019a.app

OBJECTS = feap86.o umacr6.o umatl6.o umati6.o


#OBJECTS = feap86.o 

feap: $(OBJECTS) $(ARFEAP)
        ranlib $(ARFEAP)
        $(FF) -Wl,-no_pie -o feap $(OBJECTS) \
        $(ARFEAP) -L/$(MLROOT)/bin/maci64 \
        $(LDOPTIONS) -leng -lmx
        dsymutil feap
        @@echo "--> FEAP executable made <--"

#       $(ARCHIVELIB) \
#       $(ARPACKLIB) \
#       $(ARFEAP) $(LDOPTIONS)
#       @@echo "--> FEAP executable made <--"

# UBUNTU and other GCC loader type machines
# Replace $(ARCHIVELIB) \ by:
#    -L$(FEAPHOME8_5)/packages/arpack/archive \
#    -Wl,-whole-archive -larchive -Wl,-no-whole-archive \
# Replace $(ARPACKLIB) \ by:
#    -L$(FEAPHOME8_5)/packages/arpack \
#    -Wl,-whole-archive -larpack -Wl,-no-whole-archive \

clean:
        rm -f *.o
        rm -f *genmod.mod
        rm -f *genmod.f90
        @@echo "--> Files cleaned <--"

fclean:
        rm -f feap
        rm -r -f feap*.dSYM
        @@echo "--> Feap cleaned <--"

%.o: %.F
        $(FF) -c $(FFOPTFLAG) -I$(FINCLUDE)  -I$(MLROOT)/extern/include $< -o $@

%.o: %.f
        $(FF) -c $(FFOPTFLAG) -I$(FINCLUDE) $< -o $@

%.o: %.f90
        $(FF) -c $(FFOPTFLAG) -I$(FINCLUDE) $< -o $@

%.o: %.c
        $(CC) -c $(CCOPTFLAG) -I$(CINCLUDE) $< -o $@

User Macro Commands

User Macro to reset element data

Copy one of the umacrXX.f files from the user folder to your working directory. Add the include files

include 'cdat1.h'
include 'pointer.h'
include 'comblk.h'

Set the uct variable to what you would like to name your macro (4 letters). Let's say

  uct = 'resd'

We will call the macro as resd,,ma,dl,dv where ma will correspond to our material number and dl the data location that we will change, and dv the new data value we would like to store. Now after the else place the following code

call resdsub(hr(np(25)),nint(ctl(1)),nint(ctl(2)),ctl(3))

This will pass the location of the element data arrays for all materials and our 3 command line parameters ma,dl,dv to the subroutine resdsub; the first two parameters are passed as nearest integers and the data arrays are at offset np(25) in hr. The subroutine resdsub should look like

subroutine resdsub(d,ma,dl,dv)
implicit none
include 'cdat1.h'
integer       :: ma, dl
real (kind=8) :: d(ndd,*), dv

d(dl,ma) = dv

end

User Problem Inputs

When reading user inputs from the input file it is recommended that one use a Polling Input programing style.

Memory

FEAP's memory management system is based on a fixed location in the user memory space and offsets from that location to memory blocks obtained from the operating system via calls to malloc.