PDA

View Full Version : Periodic boundary conditions in ABAQUS

roaneb
2006-07-30, 19:29
Hello All;

Does anybody know how to apply periodic boundary conditions in ABAQUS?

Thanks.

roaneb
2006-07-31, 10:59
I was able to find the equation constraint feature in which one can write equations between given sets of nodes for particular dofs. Using this, one should be able to create periodic bc's.

Jorgen
2006-07-31, 15:34
I agree, the *Equation command can be used to create periodic boundary conditions.
I have used it many times in the past, here's an example showing the compression of a foam cell:
http://polymerfem.com/polymer_files/periodicBC.png

- Jorgen

roaneb
2006-07-31, 22:26
Do you have any suggestions for applying "body forces" in the case of incompressible materials with all periodic BC's? Of course, this is using ABAQUS as well.

Thanks.

Esra

Jorgen
2006-08-01, 18:26
Are the body forces the same everywhere? If so, then you can use the *DLOAD command with for example the BX specifier.

If you apply periodic BCs for the displacements, then, depending on what you are trying to do, you might not need any "special" body force terms.

- Jorgen

FYPNoddy
2010-01-28, 13:36
Hi,

Everyone here seems to understand how to implement periodic boundary conditions to a unit cell but i am still confused. Could someone please explain this to me in more detail.

Thanks,
FYPNoddy

Jorgen
2010-02-04, 20:31
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

thisispeace
2011-01-21, 14:23
I agree, the *Equation command can be used to create periodic boundary conditions.
I have used it many times in the past, here's an example showing the compression of a foam cell:
http://polymerfem.com/polymer_files/periodicBC.png

- Jorgen

So per pair of nodes in 3D, you equate each degree of freedom? Does that usually give you a few hundred constraints?

I'm working with a honeycomb unit cell.

http://imgur.com/VLnRI.png

charmis
2011-07-28, 09:30
''in keyword *EQUATION, file "dssrtn-mod.inp", line 21607: The keyword is misplaced. It can be suboption for the following keyword(s)/level(s): assembly, instance, part''

charmis
2011-07-28, 09:33
''in keyword *EQUATION, file "dssrtn-mod.inp", line 21607: The keyword is misplaced. It can be suboption for the following keyword(s)/level(s): assembly, instance, part''

thanks

KMM
2011-09-22, 12:23
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.

matsgd
2011-09-27, 05:45
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!

Jorgen
2011-10-01, 06:27
Hej Mats, thanks for your suggestion!

-Jorgen

fatigueless
2011-10-25, 15:05
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.

Jorgen
2011-10-29, 21:36
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

Yejie Shan
2012-03-01, 04:50
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?

matsgd
2012-03-01, 07:28
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...

Yejie Shan
2012-03-02, 08:00
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.

cf99
2012-06-25, 09:05
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

brunda
2012-08-22, 06:18
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.

Brunda

matsgd
2012-08-23, 06:16
You'd have to use multi-point constraints. But the easiest way to do what you need to do is to write a piece of Matlab code in which you construct a regular, nice, mesh on the surface of the cube, and then project it down onto the sphere, layer by layer. I think it should work as both a cube and a sphere are convex.

Mats

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.

Brunda

lumpwood
2012-08-24, 03:51
Mats' idea is good. If you are using Abaqus or similar here are a few more tricks that sometimes work for circular-ish inclusions.

1) If your geometry consists of a sphere in the center of a cube then partition the geometry cell so that each face looks like the attached picture. This will allow you to use a very nice structured mesh and nodes should conform.
526

2) If the sphere is off centre in the cube use partitioning to create a smaller cube around the sphere, with the sphere at its centre. Again this should give a regular mesh.

To help ensure the mesh is repeated on all opposite faces make 8 more copies of the part and merge them to the outer faces of the original part. Mesh the resulting part, make an orphan mesh and delete the elements of the 8 copies.

3) If none of this works make membrane parts with a regular mesh for each face. Tie them to the cube faces and apply PBCs to their nodes.