Changing material properties in Steps

[MNS747]

Hi All
I am using Abaqus 6.7-1. I have a solid which is assigned Steel properties and I have three Steps. The steel properties needs to remain same for the first two steps where as it should change in the third step. I have defined two materials for this purpose named Steel-1 and Steel-2, and i want to use Steel-1 for the first two steps and Steel-2 for the third step for the same solid. I am confused how to model this and wonder if it is possible to do??? I have seen some posts but i found them confusing and would appreciate if i get any clearer help to this. Any help will be highly appreciated.

Regards

 

[mrgoldthorpe]

Define one material using a field variable. Specify a value of zero for the field variable, giving Steel-1 properties, and a field variable value of 1 for Steel-2 properties.
Specify a value of zero for the field variable initial conditions. This will use Steel-1 properties.

*INITIAL CONDITIONS, TYPE=FIELD
NALL, 0.0
(where NALL is a node set of all nodes)

In the third step set the field variable to 1:
*FIELD
NALL, 1.0

Steel-2 properties will then be used.
If there is a large change in properties (if you have plastic deformation) therte may be convergence problems.

 

[MNS747]

Thanks mrgoldthorpe
Yes it worked. your help is much appreciated.

Regards