ABAQUS Analysis: Difference between assigning Section as Plane stress/strain vs. Element type?

In ABAQUS, there are multiple ways to specif your part is in plane stress/strain. 1. When assigning the section, one can specify that it is a generalized plane strain section. 2. When assigning the section, one can specify that the section is homogeneous with a plane stress/strain thickness of 1. 3. When meshing the part, elements within the same section can be assigned an element type of generalized plane strain, plane strain, or plane stress.

I have sorted through ABAQUS documentation but have yet to arrive at a satisfactory answer, regarding the effective differences between above options.

It seems that with option 1, there is no thickness specified. Does this mean that abaqus assumes the simulation such that it is infinitely thick in the Z, as is consistent with plane strain? Versus in option 2, the thickness is 1? Meanwhile, how would results be affected if only the elements were plane stress/strain, with a regular solid and homogeneous section?

plane stress, plane strain, and generalized plane strain are three different things. In each case you need to specify the appropriate element type ( plane stress is default ).

Generalized plane strain introduces an additional issue. You must create and assign a reference point to the section. It is the reference point assignment that causes generalized plane strain to be handled separately at the section level.

A bit aside, for classical generalized plane strain you must pin the rotational degrees of freedom of the reference point. Something that is unfortunately not clear or well documented.

// other questions section thickness really only affect the scaling of edge force boundary conditions ( or reaction forces output ). If in doubt leave as 1.

Assigning any 2d element type to a 3d geometry will simply throw an error.

• Of course, I am talking about within the context of a 2d model. The point is moot in 3d, as no plane stress/strain elements can be used. Feb 25, 2018 at 23:06
• My confusion enters when a homogeneous section is chosen, and the thickness of the section is left unspecified. How does this affect the result, and how is this treated? Feb 25, 2018 at 23:08
• the default thickness is one (one unit it whatever unit system you are using). It only affects the analysis if you apply or extract edge forces (or similar things). By default your edge forces are "per unit thickness", but if you apply some actual thickness to the section, then you apply the actual force. Feb 27, 2018 at 2:03