How can I output the result to specific output variable? 1

[akadet]

Hi
I have 450 elements in my model and I would like to calculate and out volumetric strain which is ?V= ?1+ ?2+ ?3 for each element. What is the easiest way to output this kind of operation? I know I can use xy data option to operate the expression, but then i have to do it for each element before i can average them, which is tedious.

 

[xerf]

You can use CAE/Visualization->Tools->Create Field Output -> From Fields to create the field of volumetric strains.

In the dialog box select the desired step and frame.
The dialog box will list the available fields.

Then in the "Function" combo box select "Scalars".

Select the strain field. In the right side list the components of the selected strain field will be listed. Select the first normal strain component. Once selected the program will generate some code in the "Expression" edit box. This code can be edited. For example considering the LE (logarithmic strain field the generated code should be:
s2f0_LE.getScalarField(componentLabel="LE11")

You can simply copy-paste this code and modify the label "LE11" in "LE22" and "LE33" in order to obtain
something like:

s2f0_LE.getScalarField(componentLabel="LE11") +s2f0_LE.getScalarField(componentLabel="LE22") +s2f0_LE.getScalarField(componentLabel="LE33")

in the "Expression" edit box. Then press "Apply". If written correctly ABAQUS will create a new output field based on the expression you entered. This new field is placed in special step called "Session Step" and can be further treated as any other field.

There various operation which can be performed on fields and fields components. These are listed if in the "Function" combo box you select "Operators".

 

[akadet]

Hi xerf

That only works for one increment at a time, can we make it to calculate for all the increment. It can be viewed in the field output to show animation of volumentric strain for that particular step. thank you very much for your reponse.

regards,
Ed

 

[xerf]

Then you might want looking at using either UVARM user subroutine or ABAQUS Scripting Interface.