I have made a model in Abaqus program. I want to define "E" as a constant value at each node in the part.
I have entered in inp. File
*Depvar
1,
*Elastic, dependencies=1
1000., 0.25, , 1000.
6e+09, 0.25, , 6e+09
*User Defined Field
and I have entered the constant values of "E" at each node like this .
*Initial Conditions, type=Field, Var=1
Part-1 . 1 , 22980538
Part-1 . 2 , 52880552
....... and all of nodes of the part
Moreover, I have defined a subroutine USDFLD as presented in this figure.
The problem is that after calling FV1 it is not equal to the values that I have interred in this command *Initial Conditions, type=Field, Var=1......How could I Solve this problem or is there any way to define "E" at each node of the part???
Try a simpler approach: Instead of defining "E" at each node, you could try defining a uniform material property for the entire part or for specific regions within the part. This may simplify the input file and make it easier to debug any errors.
In the Visualization module, nodal values of FV1 are results of extrapolation and averaging of corresponding values at integration points and therefore may somewhat differ from the prescribed nodal values.
Hi Manar,
I think that you need to use the "Utility Routine" GETVRM* to read the Field Variable and then you can assign its value to the Statev(1). Your routine does not have a call to GETVRM, so the routine does not know the value of the Field Variable.
Regards,
Simon
* see the Abaqus manual at:
Abaqus > User Subroutines > Utility Routines > Obtaining material point information in an Abaqus/Standard analysis
To avoid using GETVARM subroutine, I need any method to enter data of "E" that I have calculated manually in ABAQUS. Do you know any method to enter specified values of "E" at each node or integration points? Simon Smith
Hi Manar,
The *ELASTIC input can be used to define the effect of temperature and field variables on the Youngs Modulus. Temperature at nodes can be defined by the user routine UTEMP, so you could define Youngs modulus to be a suitable function of temperature and the use the UTEMP to get the Youngs modulus needed at each node.
Does that help?
Regards,
Simon
Manar Naser If you are not going to change values of predefined field at material (integration) points during simulation, I think you can avoid using USDFLD. Presented .inp file (without lines pertained to USDFLD) is sufficient. From my experience, value of predefined field at any material point is equal to mean of element nodal values.
- Badges
- Science topic
- Similar topics
- Filing