# 6. ABAQUS - Boundary Conditions

## Q6.1 : How do I change the boundary conditions at some of the nodes?

Re-specify the boundary condition for only the nodes for which the boundary condition has changed with the OP=NEW option.
*BOUNDARY, OP=NEW
1, 1,,    2.5
2, 1,,    2.5
3, 1,,    2.5

In the above example the x-displacement is changed to be 2.5 units at nodes 1, 2 and 3.

## Q6.2 : How do I completely re-define the boundary conditions?

Same as above (see the answer to question 6.1).

## Q6.3 : How do I release a previously fixed d.o.f.?

Re-specify all the fixities except for the ones to be released (in the step in which these fixities are to be released) with the parameter OP=MOD.

## Q6.4 : How do I apply a prescribed displacement?

Use the keyword *BOUNDARY and in the data line specify the node number, variable (d.o.f.) number and the magnitude of the prescribed displacement. It will require one dataline per variable that is being prescribed.
*BOUNDARY, OP=NEW
1, 1,,    2.5
2, 1,,    2.5
3, 1,,    2.5
In this example nodes 1, 2 and 3 are applied a displacement of 2.5 units in the direction of the first axis (usually X axis).

## Q6.5 : Are there any normal boundary conditions like the "pinned" and "encastred" nodes that can be used?

Yes. The following is the list of named constraints.
ENCASTRE   Constraint on all displacements and rotations at a node.
PINNED     Constraint on all translational degrees of freedom.
XSYMM      Symmetry constraint about a plane of constant x coordinate.
YSYMM      Symmetry constraint about a plane of constant y coordinate.
ZSYMM      Symmetry constraint about a plane of constant z coordinate.
XASYMM      Antisymmetry constraint about a plane of constant x coordinate.
YASYMM      Antisymmetry constraint about a plane of constant y coordinate.
ZASYMM      Antisymmetry constraint about a plane of constant z coordinate.

Example :
*NGEN, NSET=FIXED
1, 10
*BOUNDARY
FIXED, ENCASTRE
Here a node set which consists of 10 nodes grouped together in node set FIXED is assigned the ENCASTRE boundary condition.
Example :
*NODE
1,  134.0,    0.0,  28.5
201,  134.0,   28.5,   0.0
**
*NGEN, LINE=C,NSET=CLAMPED
1, 201, 40
**
*BOUNDARY
CLAMPED, XSYMM

A node set called CLAMPED which consists of nodes 1, 41, ..., 201 which lie along a circular arc is first created. Then the XSYMM boundary condition is specified.

## Q6.6 : What are the variable numbers for the different nodal variables?

Following is a list of the more common variable numbers.
1,2,3 - x,y,z displacement respectively (ux, uy, uz)
1,2   - r,z displacement in an axisymmetric analysis (ur, uz)
4,5,6 - Rotation about x,y,z axes respectively  (phi_x, phi_y, phi_z)
6     - Rotation in the r-z plane for axisymmetric shells
7     - warping amplitude (for open section beam elements)
8     - Pore pressure
9     - Electric potential
11    - Temperature
12    - Second temperature (for shells or beams)
13    - Third temperature (for shells or beams)
14    - Etc.

## Q6.7 : Is it possible to connect different element types together in the same mesh ?

Yes there is no restrictions in connecting different element types together in a mesh. Any restriction you are likely to come across is inappropriate use of element types in certain analysis (procedures).

## Q6.8 : Is it possible to apply boundary conditions w.r.t. local axes?

Yes it is possible to apply boundary conditions w.r.t local co-ordinate axes. Consider the situation where you want to apply a rotation at a set of nodes which lie along the periphery of a circular arc.

Consider the figure where nodes 1 to 5 along the outer radius are to be subjected to a rotation of 1 unit. Then a local cylindrical co-ordinate system transformation is set up first. The nodes 1 to 5 are formed into an element set called CID1. The transform keyword is used to apply the transformation to the node set CID1 as follows :
*TRANSFORM, TYPE=C, NSET=CID1
0.,          0.,          0.,          0.,          0.,          1.
**
*NSET, NSET=CID1
1,       2,       3,       4,       5
**
**
** rotation boundary condition
**
*BOUNDARY CONDITION, OP=NEW
1, 5,          1.
2, 5,          1.
3, 5,          1.
4, 5,          1.
5, 5,          1.

The applied rotation is interpreted according to the transformation.

## Q6.9 : How do I ensure that the vertical displacements are the same along a line of nodes which are free to move?

Consider the situation where the nodes 1040, 1023, 1006, 989 are to have the same vertical (y-direction) displacement as node 1046. Define a a nodal set (say) VERT which includes all the nodes except for 1046. Then use the *EQUATION keyword as shown below :
*NSET, NSET=VERT
1040, 1023, 1006, 989
**
*EQUATION
2
VERT, 2, 1.0, 1046, 2, -1.0
The 2 in the second line represents the number of terms in the equation. The 2 after the nodeset and node number is the d.o.f for the y-displacement. This is folowed by the coefficient for the equation.

## Q6.10 :Is it possible to remove a specified MPC during the latter part of an analysis?

No. However it is possible to de-acivate it if using the user subroutine MPC. This is illustrated below :
Consider the situation where matching nodes in two node sets are to have the same displacements. Let a and b be such a matching set of nodes, which are in effect to be TIEd together.
If this constraint is to be in effect throughout the analysis then a MPC TIE condition could have been specified :
*MPC
TIE, a, b
Ua  =  Ub
Va = Vb
Here Ua and Va are the X and Y displacements respectively at node a.
In the ABAQUS Input file include the following statments as part of the Model.
*NSET, NSET=BASE, internal, Instance=Part-1-1, unsorted
34,  35,  36,  37,    73,   55,    56
*NSET, NSET=WALL, internal, Instance=Part-2-1, unsorted
86,  85,  84,  67,    93,  159,    96
**
....
**
*END ASSEMBLY
....
....
....
....
*MPC, MODE=DOF, USER
1, BASE, WALL
2, BASE, WALL

The User Subroutine MPC

## Q6.11 : How does one apply prescribed displacement to a node which has 3 beams which are connected through a pin joint?

The nodes are a, b and c respectively.
Use the cyclic order in specifying the MPC condition.

*MPC
PIN, a, b
PIN, b, c
Now apply the prescribed displacement to the last specified node in the MPC. ie c . The other 2 nodes a , b would have been eliminated.

This is first illustrated with a 2 beam pin joint.

If using CAE then choose the Interaction module and choose Constraint from the top line and select Manager. Click on Create....

Select MPC Constraint from the menu option and click on Continue... . Figure shows the original 2 parts. In the prompt region Select the MPC Control Point. Use the View --> Assembly Display Options... and choose the Instance tab. Untick the boxes for the other part and click on Apply.

Now click on the common point for the first part and click on Done. The message prompt will now display Select region for the slave nodes. Use the View --> Assembly Display Options... again and switch the the current part off and switch the other part into view.
Click the common point on this part. Click on Done.
In the Edit Constraint dialog box for MPC Type scroll down and select Pin and click on OK.

Now will consider the 3 beam pin joint. The method is the same up to the point of selecting the control point.
In the prompt region Select the MPC Control Point. Use the View --> Assembly Display Options... and choose the Instance tab. Untick the boxes for two of the three parts and click on Apply.

Now click on the common point for the first part and click on Done.

The message prompt will now display Select region for the slave nodes. Use the View --> Assembly Display Options... again and switch the the current part off and switch the other two parts into view. Click the common point on both parts. Click on Done.
In the Edit Constraint dialog box for MPC Type scroll down and select Pin and click on OK.

However when selecting the slave nodes take care only to select the common node. The following figure shows the possible mistake that can be made.

Here not only the common point but both beams have been selected incorrectly. Notice the colour of the beams which are both shown highlighted.

This is again noticeable when the specification of the pin joint is complete. © Cambridge University Engineering Dept
Information provided by abaqus-support
Last updated: 18 December 2011