# Thread: Periodic boundary conditions in ABAQUS

1. KMM
Member
Join Date
2008-10
Posts
36
Charmis,

It means you put keyword *Equation in the wrong place. Try to move it after keyword *Part. It works for me.
The other way you can do is create your equation in text fie, then use keyword:

kmm.
Last edited by KMM; 2011-09-22 at 12:44.

2. Member
Join Date
2006-09
Location
Sweden
Posts
81
Originally Posted by Jorgen
Periodic BC simply means that the deformation on the left size has to be the same as the deformation on the right side, etc.
That is, if the unit cells are put side by side there should be no gaps.

-Jorgen
Moreover, you can accomplish it very neatly if you introduce three dummy nodes, and let their total nine degrees of freedom represent components of the macroscopically applied deformation gradient, F (or displacement gradient, if you will). You should be able to express your constraint equations in terms of the macroscopic deformation gradient, so that you are left with imposing any macroscopic deformation on the RVE you would like, by driving the nine dofs. Now, here's the beauty of it: Since the macroscopic deformation gradient, as far as your FE model goes, is simply represented by nine numbers that the FE program believes are displacements, one might wonder what the corresponding reaction forces then are? Well, they become components of the 1st Piola Kirchhoff stress tensor, which can be turned into Cauchy stress using the F (that you have imposed). So, you never have to do any volume averaging of local stresses, etc.

Want details? See:
Journal of the Mechanics and Physics of Solids
Volume 50, Issue 2, February 2002, Pages 351-379.

Jörgen: Hoopas allt är bra med dig, och hälsa Nagi!

3. Hej Mats, thanks for your suggestion!

-Jorgen

4. Junior Member
Join Date
2011-10
Posts
1
Hi, Jorgen,

The deformed mesh shown above is cool.
I'm defining PBs in ABAQUS input file for simple tension of a 3D cell, the stress seems to be unreasonable. Maybe because of the rigid motion? Did you apply other constraints in your compression example with periodic BC? Hopefully I can discuss with you to figure it out.
Last edited by fatigueless; 2011-10-25 at 15:07.

5. No I did not specify any other specific boundary conditions. If you still have problems then I recommend that you checkout the article by matsgd mentioned above.

-Jorgen

6. Junior Member
Join Date
2012-03
Posts
10
Hi, Jorgen

I am modelling a periodic structure these days and I've encountered some problems. Here are two of them:
1.I want to use Equation constraints to achieve PBC of RVE. Take a 2D square box for example(tension in direction 1):
**Make relative displacements(direction 1) between left nodes and right nodes equals displacement of reference point.
*Equation
3
Nodesets_left, 1, 1
Nodesets_right, 1, -1
Nodesets_refencepoint, 1, -1
**Make relative displacements(direction 2) between left nodes and right nodes equals zero.
*Equation
2
Nodesets_left, 2, 1
Nodesets_right, 2, -1
**Make relative displacements(direction 1) between top nodes and bottom nodes equals zero.
*Equation
2
Nodesets_top, 1, 1
Nodesets_bottom, 1, -1
**Make relative displacements(direction 2) between top nodes and bottom nodes equals zero.
*Equation
2
Nodesets_top, 2, 1
Nodesets_bottom, 2, -1

Then I met the error:XXXX nodes are missing degree of freedoms........It confuses me. I don't know the reason and the way to solve it.
2.In the *Equation constraints above, I used nodesets instead of single node, but labels of nodes in each sets are often not in consistence, so is there some way convenient to make the nodes in specific order as one wish?

7. Member
Join Date
2006-09
Location
Sweden
Posts
81
Originally Posted by Yejie Shan
Hi, Jorgen

I am modelling a periodic structure these days and I've encountered some problems. Here are two of them:
1.I want to use Equation constraints to achieve PBC of RVE. Take a 2D square box for example(tension in direction 1):
**Make relative displacements(direction 1) between left nodes and right nodes equals displacement of reference point.
*Equation
3
Nodesets_left, 1, 1
Nodesets_right, 1, -1
Nodesets_refencepoint, 1, -1
**Make relative displacements(direction 2) between left nodes and right nodes equals zero.
*Equation
2
Nodesets_left, 2, 1
Nodesets_right, 2, -1
**Make relative displacements(direction 1) between top nodes and bottom nodes equals zero.
*Equation
2
Nodesets_top, 1, 1
Nodesets_bottom, 1, -1
**Make relative displacements(direction 2) between top nodes and bottom nodes equals zero.
*Equation
2
Nodesets_top, 2, 1
Nodesets_bottom, 2, -1

Then I met the error:XXXX nodes are missing degree of freedoms........It confuses me. I don't know the reason and the way to solve it.
2.In the *Equation constraints above, I used nodesets instead of single node, but labels of nodes in each sets are often not in consistence, so is there some way convenient to make the nodes in specific order as one wish?

There's an "unsorted" option when you define node sets. It means that the node numbers will be stored in the order you specify them.

Can you introduce line breaks in an equation like that? Perhaps you can, but I did not know...

8. Junior Member
Join Date
2012-03
Posts
10
Originally Posted by matsgd
There's an "unsorted" option when you define node sets. It means that the node numbers will be stored in the order you specify them.

Can you introduce line breaks in an equation like that? Perhaps you can, but I did not know...
Thank you for your good avice, matsgd!
I have refered to Abaqus user's manual and now I'm wondering whether this could be achieved in CAE or can unsorted node sets only be defined in Input files? I didn't find any option for defining unsorted node sets in CAE..
As for line breaks you mentioned, I have to admitted that I was too careless.. I typed those stuff directly on the forum and forgot to add the commas.

9. Junior Member
Join Date
2012-06
Posts
1
Hi, i am pretty new to this topic, but i also want to use a perioic BC for a simple geometry.
But i have some difficulties with the DOF...
If i select all Nodes (on the edge) and have a equation for every node, isnt the system overdetermined?

I wrote a Makro to generate a Node and constraint list... but when i use this list with Abaqus i get an error where three nodes have no DOF...

The Input looks like this:

** Constraint: top_bc2-x
*Equation
4
top_bc2,1,1.
top_bc3,1,-1.
bottom_bc2,1,-1.
bottom_bc3,1,1.
** Constraint: top_bc2-y
*Equation
4
top_bc2,2,1.
top_bc3,2,-1.
bottom_bc2,2,-1.
bottom_bc3,2,1.

top_bcX defines a node and bottom_bcX is the opposite node

So i get (N1-N2)|top -(N1-N2)|bottom = 0 (for x and y)

This should provide a BC.

I hope my equation is okay?! Or maybe this is the problem.

@Jorgen
The result should look like your picture.

thanks for any tip.

Christoph

10. Junior Member
Join Date
2009-10
Location
Kanpur, India
Posts
23
Dear Jorgen,

I have a cube with a spherical inclusion at the center. Without the inclusion, I have successfully applied periodic boundary conditions. However, with the inclusion in place, the mesh is not exactly uniform on cube faces and hence nodes are not ordered and this is making the use of *Equation very difficult.

Is there a work around this?

Considering two opposite parallel faces say the top and bottom:
I have read the following in the literature: create a *Copy of the bottom face and translate it closer to the top face and apply *tie constraint. And apply *Equation constraint between the bottom face and its copy. (read in the literature)

But I do not understand how to create a face and translate too? I have looked up manuals with much success. Any kind of guidance would really help.