# Enhanced strain formulation for plane strain 2D analysis

Hi everybody,

I started another discussion yesterday on the same analysis, but this time the problem is

slightly different: i have a 2D geometry and i want a plane strain state. I click on the "plane strain" window as in the following figure

But after that on the result i still get a Z strain.

I read on the "solution information" that my element (PLANE182) has KEYOPTION(1)=2 which means "Enhanced strain formulation" which occasionally add a degree of freedom to avoid shear Locking.

Well, what if the strain along Z is due to the addition of UZ DOF?

If yes, how can i solve this problem? I just want Plane strain from my solution, that's the objective.

Thank in advance! I will appreciate any help

## Comments

I doubt that the use of the enhanced strain formulation is the cause of your problem. Those internal degrees of freedom help to also capture bending stress that linear elements are known to be bad at.

Now back to your question, you can change the element technology by setting the following:

!TURN OFF AUTOMATIC SELECTION OF ELEMENT TECH

ETCONTROL,OFF, ON

!SET THE ELEMENT TO PLANE 182 WITH WITH FULL INTEGRATION

ET,MATID,PLANE182

KEYOPT,MATID,1,0

!SET THE BEHAVIOUR TO PLAIN STRAIN

KEYOPT,MATID,3,2

maybe if you share more details about your problem and show geometry and BC, i ca better understand your problem.

Thank you a lot for the APDL command and for the fast reply.

However i still get strain along Z. Do i have to insert the APDL command on the geometry of the body?

The problem is a 2D disk (i'm really sorry i'm not allowed to share pics of the problem despite is very simple) and in transient structural i'm evaluating the circumferential stress of the disk with the time.

The load comes from a thermal transient analysis in fluent, i export the thermal field for each time-step. The stress comes from the temperature gradient along the radius of the disk.

As i said i need to get plain strain from this analysis, so the strain along z (normal direction of the plane) has to be zero. I also tried to make the mesh in APDL and then exporting it to workbench, but it did not work.

No constraints are applied.

I solved the problem by modifying the material model: i changed the coefficient of thermal expansion from isotropic to orthotropic by putting the coefficient of thermal expansion along z equal to zero. In this way i do not get any thermal expansion along the normal direction and so thermal strain. As i read in literature the stress sigma has to be non-zero and is what i get.

Could this be correct?

Hello,

Glad to know you have solved your problem. I think what you have done is correct. In the apdl theory reference (page 6, v19.2) , you will find that ansys allows for different coefficient of thermal expansion in the element basis direction so i suspect that by using the orthotropic option and setting that coefficient to zero in z direction, no thermal strains are generated in that direction. That makes sense to me.

You are correct, the stresses in the plain strain are nonzero in z direction. at least for linear elasticity you can check this from elementary calculations.