Dear Negar Kamali,

I think you can use degrees of freedom 1 to 6 and assign them to your nodal variables without causing any problem.

As you mentioned, Abaqus uses the following convention for the degrees of freedom:

1 : Translation in direction 1

2 : Translation in direction 2

3 : Translation in direction 3

4 : Rotation about the 1-axis

5 : Rotation about the 2-axis

6 : Rotation about the 3-axis

...

11 : Temperature

However, I think the above convention is not important when you define your own element using UEL.

I had a case for which I had 3 degrees of freedom (displacement in x-direction, displacement in y-direction, and rotation about z-axis). Therefore, I used DOF 1, 2, 6 in my UEL. To make sure that such a convention is not of importance in UEL, I ran the same UEL code with DOF 1, 2, 3 and I got exactly the same results.

In another case, my colleague had 4 DOF (displacement in x-direction, displacement in y-direction, rotation about z-axis, and Lagrange multiplier), and he used DOF 1, 2, 6, 9. Note that based on the Abaqus convention, DOF 9 is assigned to electrical potential. However, using DOF 9 for the Lagrange multiplier did not cause any problem.

All in all, it seems that in UEL, Abaqus convention is not important and you only need to correctly define AMATRX and RHS according to your formulation.

In order to define your DOF, you can use the following line in your input file (this is what I used for my case):

--------------

*USER ELEMENT, NODES=8, TYPE=U2, PROPERTIES=7, COORDINATES=3, VARIABLES=32

1, 2, 6

--------------

NODES : number of the element nodes

TYPE : Un in Abaqus/Standard and VUn in Abaqus/Explicit

PROPERTIES : number of properties defined in UEL subroutine

COORDINATES : maximum number of coordinates needed in UEL (I had 3 but for your case it should be 6)

VARIABLES : number of solution-dependent state variables

(first line) : list of active degree of freedom ( I used 1, 2, 6 but I think for your case it should be 1, 2, 3, 4, 5, 6)

Regards,

Dear Farid,

thanks for your comprehensive response. It is a relief to know that it's possible to use one's own convention for dofs in ABAQUS, but I'm just curious . When I look into my msg file, for dofs 4-6 , ABAQUS has used momentum equations to solve for rotations, 

Somehow I can not add any words above, so I continue here: 

When I look into my msg file, for dofs 4-6 , ABAQUS has used momentum equations to solve for rotations, and even the units are different, how the responses would correspond to displacement? 

I also used dofs 1,2,12,13,14,15 and noticed that in msg file, there are no info regarding the dofs 12-15! and the responses were slightly different! 

considering your comments, ABAQUS' dofs are not reserved and we can always overwrite them, Thanks again.

Bests

Dear Negar,

I think the slight difference which you get is due to your boundary and loading conditions.

Let me explain it on my case in details. 

As I mentioned, I had 3 degrees of freedom (displacement in x-direction, displacement in y-direction, and rotation about z-axis). Therefore, I used DOF 1, 2, 6 in my UEL. As a simple example, I would like to model a cantilever beam where all nodes at the left boundary are clamped (ENCASTRE) and a vertical concentrated load is applied on the top node at right side of the beam. When I use "ENCASTRE" condition for the nodes at the left side of the beam, it means that DOF 1,2,3,4,5,6 will have zero value. Similarly, when I use "CLOAD" to apply the vertical concentrated load on the top node at right side of the beam, I should  use "2" along with "CLOAD" for the direction of the load.

Now, instead of DOF 1, 2, 6, I would like to use DOF 4, 5, 6 in my UEL. To this end, I need to use "5" along with "CLOAD" for the direction of the load (Not "2").

For your case, I would expect you to get different results when you use DOF 1, 2, 12, 13, 14, 15 instead of DOF 1, 2, 3, 4, 5, 6 because your boundary and loading conditions can be only applied for DOF 1 to 6 and when you use any DOF higher than 6, you are not applying any conditions on it. Therefore, I think it would be better if you use DOF 1 to 6. Also, make sure that your applying boundary and loading conditions are exactly consistent with your selected DOF and your own formulations.

I hope that helps,

Regards,

Dear Farid,

thanks again! your comments really help.I appreciate it

. Actually when I use dof 1,2,14,15,16,17 and I apply boundary conditions on  14,15,16,17 , Abaqus applies it and gives me the correct response which is zero exactly for those I want. (it is not correct for the nodes without BC) that part of my input file is something like this :

------------------------------------------------------------------

** Name: BC-4 Type: Displacement/Rotation

*Boundary

_PickedSet16, 2, 2

*Boundary

_PickedSet16, 15, 15

*Boundary

_PickedSet16, 17, 17

** Name: BC-5 Type: Displacement/Rotation

*Boundary

_PickedSet18, 1, 1

*Boundary

_PickedSet18, 14, 14

*Boundary

_PickedSet18, 16, 16

--------------------------------------------------------

and the same for the lode. In ABAQUS' documentation for UEL, they have following statement:

The activated degrees of freedom should follow the Abaqus convention (“Conventions,” Section 1.2.2). In Abaqus/Standard this is important because the convergence criteria are based on the degrees of freedom numbers. In Abaqus/Explicit the activated degrees of freedom must follow the Abaqus convention because these are the only degrees of freedom that can be updated.

What is your opinion on this?

Also, I noticed something in the line you wrote:

--------------

*USER ELEMENT, NODES=8, TYPE=U2, PROPERTIES=7, COORDINATES=3, VARIABLES=32

1, 2, 6

--------------

you have 8 nodes on your element and for each node you have 3 degree of freedom, totally 24 dof per element, am I right? right now I want to have 4 nodes and 6 dof per node, so my input line is like this:

*USER ELEMENT, TYPE=U1, NODES=4, COORDINATES=2, VAR=16,

INTEGRATION=4, TENSOR=PSTRAIN, PROPERTIES=1

1,2,14,15,16,17

Is it correct? What concerns me now, is that we maybe using different terminology here!  (nodes and degree of freedoms)

Thanks a lot for your help

Dear Negar,

As you noticed, I have an element with 8 nodes where each node has 3 DOF resulting in total 24 DOF. However, what I mean by DOF in my previous comments is only DOF of one node (3) not DOF of one element (24).

I might be mistaken, but my UEL results show that we can overwrite DOF at least in my case. Let me explain my interpretation of how Abaqus works:

Assume that we have a nonlinear problem (like elasto-plastic material nonlinearity).

In UEL we should provide Abaqus with AMATRX (stiffness matrix or element tangential stiffness matrix) and RHS (right-hand-side vector). 

As nonlinear problems need to be solved iteratively, Abaqus applies the external force incrementally. In each force increment, Abaqus performs iteration until the convergence criterion is satisfied. Therefore, we have the following simplified algorithm:

 Loop #  1 : load increment

          Loop # 2 : iteration for the load increment

                          you define : AMATRX=[B]T*[Cep]*[B}

                          you define : RHS=-[B]T*{Stress}

                          Abaqus solves linear problem [AMATRX]*{dU}={RHS}

                          Abaqus updates {U}={U}+{dU}

                          Abaqus checks the convergence criterion

         End Loop # 2

End Loop # 1

Generally speaking, the convergence criterion is the one which shows the difference between external applied force vector {Fext} and internal force vector {Fint}.

Abaqus gets {Fext} from your input file as you define the boundary and loading conditions in the input file.

Abaqus gets {Fint} from your UEL as you define RHS and AMATRX.

As soon as the norm of difference between {Fext} and {Fint} becomes less than the convergence tolerance, the convergence criterion is satisfied and Abaqus starts the next load increment.

In all of the above procedure, you will see that the Abaqus convention does not play any role (this is my interpretation). Abaqus just divides your external load into couple of increments, then for each increment Abaqus solves the linear system of equations [AMATRX]*{dU}={RHS} and then calculates the difference between the external and internal force vectors as the convergence criterion. 

Regards,

Dear Farid,

what you're suggesting seems completely logical. I will proceed without being worried about my dofs and I will write here if I encountered any problem with them, in order to discuss further. Thanks for all the explanations and help.

Negar

Dear Negar,

did you use the rotation dofs 4~6 in the uel/vuel?

now, I'm programing a linear flat shell element Q4 in vuel, but the incremental strains ([B_Bending] * {du_rotation}, [B_TransverseShear] * {du_w, du_rotation}) are incorrect.

It looks like the incremental rotation is not additive and different from incremental displacement.

From the manual 32.15.1, it says: 

Rotation update in geometrically nonlinear analyses

If all three rotational degrees of freedom (4, 5, and 6) are used at a node in a geometrically nonlinear analysis, Abaqus assumes that these rotations are finite rotations. In this case the incremental values of these degrees of freedom are not simply added to the total values: the quaternion update formulae are used instead. Similarly, the corrections are not simply added to the incremental values. The update procedure is described in “Rotation variables,” Section 1.3.1 of the Abaqus Theory Guide, and is mentioned in “Conventions,” Section 1.2.2.

To avoid the rotation update in a geometrically nonlinear analysis in Abaqus/Standard, you may define repeated node numbers in the nodal connectivity of the element such that at least one of the degrees of freedom 4, 5, or 6 is missing from the degree of freedom list at each node.

Regards,