Plane strain elements work incorrectly in rolling process 2

[polak7]

When I use plane stress elements in simulation all works great. The picture below shows the results from my analysis with the use of that elements:

But when I change the type of elements to plane strain, the results are terrible. Look:

The only change I did is different element type. And results are completely confusing. Why the slab returns to its oryginal shape after it exits the roll gap?
Is it possible to fix it? I have to use plane strain elements.

 

[corus]

Look at the stresses that are being produced. The plastic behaviour of the elements will depend upon the calculated stress intensity. You can think of that as being the maximum of the principal stress differences. With plane stress elements, one principal stress component will be zero. With plane strain elements it may be that the out of plane stress has the same sign as the other two components such that the stress intensity is reduced and may be less than yield and elastic. With plane stress elements, and one zero component, the stress intensity will be larger and perhaps above yield and so shows plastic behaviour. Or you've made a mistake in your input for material properties.

 

[polak7]

You are right corus, something is wrong with stresses. Look at the pictures below:

Plane stress:
S11:

S22:

Strain intensity:

And plane strain:
S11:

S22:

S33:

Strain intensity:

How can I fix it?

 

[corus]

If you have temperatures as part of your loading then plain strain will give you a high stress, unless you use generalized plane strain elements to allow out of plane expansion. As I said earlier, your maximum compressive stresses are roughly all the same value in all directions and so your stress intensity will be small and below yield stress, hence no yielding. Note that there are methods for calculating the stresses or roll separating force during rolling with which you can compare with:

http://www.me.umn.edu/courses/old_me_course_pages/me3221-sum/Overviews/Rolling/rollingforce.html

for example. Search for Sims formula too.

 

[polak7]

Ok I think that I understand the theory, thanks. I have changed section to generalized plane strain and I defined reference points on my two parts (Slab consists four layers built by those two parts, as have been shown in picture below)

But when I start the analysis, solver returns errors:
SOLIDSECTION REF. NODE 1204 INSTANCE Core material layer-1 IS NOT ACTIVE IN THIS MODEL
SOLIDSECTION REF. NODE 1204 INSTANCE Core material layer-2 IS NOT ACTIVE IN THIS MODEL
SOLIDSECTION REF. NODE 4805 INSTANCE Transition Layer-1 IS NOT ACTIVE IN THIS MODEL
SOLIDSECTION REF. NODE 4805 INSTANCE Transition Layer-2 IS NOT ACTIVE IN THIS MODEL

I have tried to define reference poins in the middle of the layers too, but errors did not disappeared.
What should I do?

 

[corus]

Not sure why you have 4 reference points, or 4 parts for that matter, unless you have contact between each of the parts. If the slab is assumed to be a solid with 4 materials then simply have one part partitioned into 4 to which you assign different materials and section properties. The reference point should only be restrained rotationally for which you have to manually edit the .inp file (freedoms 5 and 6 of I recall). Usually if a node is not active in the model it means you have the node on a contact surface and the freedoms have been removed, for which you're then trying to restrain.

 

[polak7]

Slab consists 4 instances, which are built from 2 parts. Each part is a different material. So, I have 2 copies of each part in the assembly. I have to put different mesh density on them, that's why I did not partitioned one part into 4. It is much easier to adjust meshes in that way. Instances are tied each other.
I have never had to deal with input files, so I will stop now with this problem. First, I have to learn about working on input files.
So, thank you for your help corus. Maybe I will refresh this thread in the February.