kinematic coupling wont work if these nodes are separated by some distance. Your best bet will be either linear equation constraint (you need to be careful here) or connectors element (join or link). Alternatively you can also check PIN constraint

Abhimanyu,

Thanks for the answer. All the nodes lie on a single plane. Could you explain why the kinematic constraints wont work ?

I assigned one of the nodes as the reference node and enforced a kinematic constrain between the ref node and rest of the nodes.

Thanks.

Kinematic coupling is more like rigid body constraint (with slight twist)...just for an exercise and it'll make my point clear (extremely easy to generate such input file):

Yeah, if you just want to constrain one DOF, they I'd just use an EQUATION constraint.

You can probably also use MPC, TIE

@Martin, I guess MPC or Tie constraints doesnt have a specific DOF control.

All my nodes are on a single surface of a cube, I am imposing the displacements so that the entire surface moves as a whole in x direction although each of the nodes can have differential displacement in y .

@Abhimanyu, I didn't understand your exercise. let me explain the problem.

I have a cube which is loaded in y, i would like to impose uniform poisson contraction on x and z faces ( as my cube is a polycrystal and doesnt have uniform posson contraction).

The MPC link or pin constraint, to my understanding, maintians the distance between the nodes same but I dont need that. i need to constrain displacements only in x and not in y.

I tired using the linear constraint equation between 1 node of the surface and rest of the nodes but it is not converging.

Additionally, check out these benchmark problems and how *EQUATIONS are used in Section 3.1.5 Fitting of elastomeric foam test data (http://50.16.225.63/v2016/books/bmk/ch03s01ach171.html). If you have more than one element you just need to make sure the entire face moves together, so you need to create a node set will all the nodes on the face, minus the one master node, for the equation constraint.

@Abhimanyu , Thanks I shall check that.

@Mike: Yes, thats exactly what I did.

I have attached a pdf file to explain what I have done

Note : I am running crystal plasticity simulations using an UMAT

What is there a million elements in that?? Please make sure it is not the umat causing this lack of convergence. Try using a simpler mesh with a built in linear elastic material first. Then add your umat and let us know how it goes.

Yes, there are millions of elements. I am trying to do it on a simple mesh with linear elastic as Abhimanyu suggested. I shall get back after I run. Thanks!

Sounds good - you probably know about these references, but  "Parsons, E., PhD thesis, MIT, 2006." has a good framework described to get macroscopic behavior for this stuff.  Another reference is Danielsson, M., Parks, D.M., Boyce, M.C., J. of the Mechanics and Physics of Solids, 50, 351-379, 2002.

Few things I noticed:

Have fun :)

Abhimanyu and Mike :

Thanks for your inputs and help, really appreciate it!

I have run a very simple model with isotropic material properties and it seems to work.

@Abhimanyu, the UMAT is a very well tested one and it has been in use for at least 3 years. I have succesfully obtained results with a slightly different BC's from what I am trying.

Bcs with which I obtained results :

@Face X=0 , Ux=0

@Face X=width, Free ( No displacements imposed)

@Face Y=0 , Uy=0

@Face Y=width, Uy is specified

@Face Z=0 , Uz=0

@Face Z=width, Free ( No displacements imposed)

Why is the choice of a master node not right ? Could you please educate me with this ?

Also I have attached the .inp file with displacements obtained.

Thanks,

Prithivi

I can't see any constraint being imposed on x or z face in your input file!!!

To understand why your choice of master is not the best one, read abaqus analysis manual regarding equation constraint carefully.

Apologies, .inp updated

When I said "your choice of master node is not the best one" because it'll limit your freedom. How? read manual for equation constraint :)

This is the Abaqus manual content I have read few times but I couldn't still find the answer.

I found these sentences relevant but still not very sure :

"In Abaqus/Standard the first nodal variable specified ( corresponding to ) will be eliminated to impose the constraint (in the above equation constraint, degree of freedom 3 at node 5 will be eliminated); therefore, it should not be used to apply boundary conditions, nor should it be used in any subsequent multi-point constraint, kinematic coupling constraint, tie constraint, or equation constraint (see “Kinematic constraints: overview,” Section 31.1.1). In addition, the coefficient should not be set to zero"

My first nodal variable is one of slave nodes and not a master node.

http://abaqusdoc.ucalgary.ca/books/usb/default.htm?startat=pt08ch31s02aus117.html#usb-cni-pequation