The conventional theory of mechanism-based strain gradient plasticity is realized via ANSYS user programmable features for USERMAT subroutine.
Strain gradient plasticity is a theory of continuum solid mechanics which aims at modeling the irreversible mechanical behavior of materials, with specific focus on metals and on their response at appropriately small size, typically on the order of micrometers or less. For small scale, a variation in size leads to a peculiar effect, denoted as “smaller being stronger.” At the crack tip, taking into account gradient plasticity leads to a significant increase of stresses.

In source files you can find a APDL script example for 2D cracked body. After compiling and attaching present dynamic link library as ANSYS user material copy and run this file from ANSYS Mechanical command line.
If you using this code for research or industrial purposes please cite one of the following publications.

• Crack tip fields and fracture resistance parameters based on strain gradient plasticity

• Mode I and mode II stress intensity factors and dislocation density behaviour in strain gradient plasticity

• Inversion of dislocation densities under mixed mode fracture

I want to say thank a lot to Emilio Martínez Pañeda for the detailed presentation of his methods in open acsess and active assistance. This helped a lot in the implementation of CMSG theory into ANSYS. This project is reworked his ABAQUS subroutine described here.

Install Visual Studio first and then Intel fortran compiler. When installing the compiler, select "Integrate into Visual Studio". Supported versions can be found in the ANSYS documentation in the section on User Programmable Features (UPF). Add LIB and INCLUDE variables in the system environment. Create new solution and add new fortran dll project. The name of the created library must be "USERMATLIB.DLL". Add all fortran files from Source directory to your dll project. Tune compiler according to instructions present below. After compiling connect library to ANSYS.

After creation the dll file you have to connect this library to ANSYS:

1. Create environment variable named ANS_USER_PATH

My Computer->Properties->Advanced system settings->Advanced

On the tab, click on the button:

Environment Variables->System Variables->New

2. In the variable value field, specify the path to the folder where library is located. Use only latin characters in the path.

For example:

C:\Username......\Usermatlib

If everything is connected correctly in the ANSYS output window at startup there will be a line

User link path <ANS_USER_PATH>: *path to your folder*" 

3. After launching the ANSYS, create an user material

Preprocessor->Material Props->Material models

4. In the drop-down list of materials, select

Structural->Specialized Materials->User material options->user material

And add cells. There should be 6 properties in total. Of which:

In command line it will be looks like present bellow

!* Define parameters related to CMSG model
!* Modulus of Elasticity
Young = 200000
!* Poisson ratio
nu = 0.3
!* Yield Strength
S02 = 300
!* Length parameter in the CMSG model (approximate order 1e-6 meters)
Leng = 1E-6
!* Strain hardering exponent (0 < N < 1)
SHE = 0.15
!* Flag 0 or 1. Usually 1 for metals
Flag = 1

!* add user model
TB,USER,1,1,6,
TBTEMP,0
TBDATA,,Young,nu,S02,Leng,SHE,Flag

5. Add 13 state variables

Preprocessor->Material Props->Material models->Structural->Specialized Materials->User material options->State Variables

APDL script for preprocessor section

TB,STAT,1,1,13,
TBTEMP,0
TBDATA,,0,0,0,0,0,0
TBDATA,,0,0,0,0,0,0
TBDATA,,0

6. Access to user variable arrays

Before starting on the solution in the solver (/SOL) in the command line of ANSYS, write the line:

• to save every substeps results

OUTRES,SVAR,ALL

• to save only the last step

OUTRES,SVAR,LAST

In order for all elements of user arrays to be available, command GRAF must be used in the postprocessor (/POST) section.

/GRA,FULL

That's all. Further we work as with the usual scheme.

*** - your version of ANSYS.
All other settings by default. Its allows me connect to ANSYS for debugging.