Ansys Constraints and Loads

Constraints and loads are defined in the Solution section. The symbol D is used for any general type of nodal constraint and the symbol F is used for any general type of applied nodal action. This derives from the concept of F = Kd. Distributed loads are defined with several different symbols. For example, SF is a surface force applied at nodes with SFBEAM for beams in particular.

The Constraint: A constraint is defined with the D command. Constraints include not only roller, pin, and fixed supports in mechanical systems, but also things like voltage and temperature for other types of analyses. There are at least three options that follow these commands. They are separated by a comma.
1. The node number where the constraint is applied
2. The constraint type
  - UX for translation in the X direction
  - UY for translation in the Y direction
  - UZ for translation in the Z direction
  - ROTX for rotation about the X axis
  - ROTY for rotation about the Y axis
  - ROTZ for rotation about the Z axis
  - ALL for all six of the above
  - VOLT for voltage
  - TEMP for temperature
3. The value. This is usually zero for structural analysis, but is the voltage or temperature in others cases.
4. Additional constraints can be given starting with the seventh option with commas setting off default values
The commands looks like this:
```
        D,1,UY,0         ! constrain node 1 in y direction (roller)
        D,3,UX,0,,,,UY   ! constrain node 1 in x and y direction (pin)
        D,1,ALL          ! constrain node 1 all 6 degrees of freedom
        D,1,VOLT,20      ! voltage of node 1 is 20
        D,2,TEMP,300     ! temperature of node 2 is 300
```
Constraints can be applied to a set of regularly spaced nodes by using the fifth and sixth options. As with the Load command, the fifth option is the last node number in the series and the sixth option is the node increment between the loads. For example, the lines:
```
        nrows = 5                      ! number of element rows
        D,1,TEMP,400,,(nrows*10+1),10  ! temp of inside nodes
```
constrain the temperature to be 400 at nodes 1, 11, 21, 31, 41, 51.
The Concentrated Load: A concentrated load is defined with the F command and has at least three options.
1. The node number where the load is applied
2. The load type
  - FX for a force in the X direction
  - FY for a force in the Y direction
  - FZ for a force in the Z direction
  - MX for a moment about the X axis
  - MY for a moment about the Y axis
  - MZ for a moment about the Z axis
3. The value of the load.
The commands looks like this:
```
        F,1,FX,1000      ! force X direction at node 1
        F,4,FY,-20e3     ! force -Y direction at node 4
        F,1,MX,4e3       ! moment about X axis at node 1
        F,2,MZ,42e3      ! moment about Z axis at node 2
```
Loads can be applied to a set of regularly spaced nodes by using the fifth and sixth options. The fifth option is the last node number in the series and the sixth option is the node increment between the loads. For example, the line:
```
        F,1,FY,-1000,,5,2
```
applies a downward 1000 force at nodes 1, 3, and 5. Notice the double comma after 1000.
The Distributed Beam Load: A distributed load on a beam is defined with the SFBEAM command, which has at least four options. The first option is the element number where the load is applied. Use ALL when the load applies to all selected elements. The second option is 1 while the third option is PRES, for pressure. The fourth option is the pressure value that applies uniformly throughout unless there is a fifth option. The fifth option specifies the pressure at the other end of the element to designate a tapered load. The command looks like this:
```
        SFBEAM,1,1,PRES,60    ! uniform load 60 lb/in
        SFBEAM,1,1,PRES,0,60  ! tapered load 0-60 lb/in
        SFBEAM,2,1,PRES,60,0  ! tapered load 60-0 lb/in
        SFBEAM,ALL,1,PRES,60  ! uniform Load 60 lb/in
```
The first line creates a uniform load of 60 on the first element while the second gives a tapered load from 0 to 60 on the first element. The third command puts a load tapered from 60 to 0 on element 2 while the fourth command loads all selected elements uniformly with 60.
The General Distributed Load: A distributed load from pressure or thermal convection can be defined in several ways. The most general way is with the SF command, which has at least three options depending on the type of load. The first option is the node number where the load is applied. Use ALL when the load applies to all selected nodes. The second option is PRES for pressure or CONV for thermal convection. The third option is the pressure value for PRES. For CONV, the third option is the convection coefficient and the fourth option is the ambient temperature. If the pressure or temperature apply to only some of the nodes, you must select the nodes first with the NSEL command. For example:
```
        NSEL,S,NODE,,9,49,10    ! select top nodes
        SF,ALL,PRES,pressu      ! load on upper surface
        NSEL,ALL                ! reselect all nodes

        SF,ALL,CONV,0.2,70
```
the first NSEL command starts a new selection set with the S option. The second option specifies that nodes are to be selected. The next option is the default. The fourth and fifth options specify that node 9 is the first and node 49 is the last in the set. The sixth option increments the node numbers increment by 10. Therefore the selected nodes are 9, 19, 29, 39, and 49. The second command applies to the selected nodes, a pressure defined previously by pressu. The third command reselects all nodes. The fourth command applies a convection load to all selected nodes using a convection coefficient of 0.2 and a temperature of 70.

MENG 421 -- Source Program -- Ansys index -- Class assignments