The UMAT problem with no strain and stress

Dear Atefe Geramian

You should be able to visualize the stress components. However, notice that you will never be able to visualize the strain components, among other variables, because they are not assigned to any variable in the subroutine that is given back to ABAQUS. You will need to store them in the STATEV variables for that. 

You can find more information regarding this issues in the documentation.

Best regards,

Emilio Martínez Pañeda

SIMUMECAMAT Research group
www.simumecamat.com

Hi,

There might be multiple reasons for this problem. Please use some WRITE statements and see whether you get proper numbers for the variables that are updated inside UMAT. If the variables returned back to abaqus from UMAT such as STRESS, DDSDDE, STATEV etc by chance turns (NAN) inside the subroutine, then there is probability that these errors come. 

"The selected primary variable is not available in the current frame for any elements in the current display group"

Thanks and Regards,

Rohith

It might be helpful to know what model you want to code.

Mind that

STATEV(4)==0

is a test that works exclusively if statev(4) is an integer.

Study these chapters in the manual (section numbers depend on release of your Abaqus !):

13.2.1 USER SUBROUTINES: OVERVIEW

Testing and debugging
When developing user subroutines, test them thoroughly on smaller examples in which the user
subroutine is the only complicated aspect of the model before attempting to use them in production
analysis work.
If needed, debug output can be written to the ABAQUS/Standard message (.msg) file using
FORTRAN unit 7 or to the ABAQUS/Standard data (.dat) file or the ABAQUS/Explicit status (.sta)
file using FORTRAN unit 6; these units should not be opened by your routines since they are already
opened by ABAQUS.
FORTRAN units 15 through 18 or units greater than 100 can be used to read or write other userspecified
information. The use of other FORTRAN units may interfere with ABAQUS file operations;
see “FORTRAN unit numbers used by ABAQUS,” Section 3.6.1. You must open these FORTRAN units;
and because of the use of scratch directories, the full pathname for the file must be used in the OPEN
statement


also:
3.6.1 FORTRAN UNIT NUMBERS USED BY Abaqus
Abaqus uses the FORTRAN unit numbers outlined in the table below. Unless noted otherwise, you should not try to write to these FORTRAN units from user subroutines.
For Abaqus/Standard, you should specify unit numbers 15–18 or unit numbers greater than 100 .
For Abaqus/Explicit, specify units 16–18 or unit numbers greater than 100 ending in 5 to 9, e.g. 105, 268, etc. You cannot write to the.sta file.




Here is an example to write to a self-defined file:

IF (condition fulfilled) THEN
   open(15,file='Exp.rpl',position='append')
   write(15,*) TIME(2), RPL
   close(15)
END IF

I do not remember right now if 'Exp.rpl' is to be preceded by the full path to the file.

To write to the log file:
IF (condition fulfilled) THEN
    print*, NDI
END IF


Good luck

Frank

Try to check the values in your input file. I faced the same error because I entered a value of zero for stiffness by mistake.