0

A question in ABAQUS (may seem very basic). How to apply concentrated force or line load at an angle in ABAQUS? ABAQUS only gives option to specify components in X, Y, Z directions for a concentrated force. So resolving force is only option? Can anyone comment?

user3519733
  • 79
  • 2
  • 9

2 Answers2

1

It's a simple matter of understanding that force is a vector quantity. Given known angle(s), calculate the components in the coordinate system of choice.

You might really be asking "If I know that my force is normal to a surface in its local coordinate system, how do I calculate its components in global (x, y, z) system?"

If that's your real question, it's just a vector transformation from the surface normal coordinate system to the global (x, y, z). The surface coordinate system should be (n, t, z) where n = unit vector normal to the surface, z = unit vector out of the plane, t = unit vector tangential to the surface defined by the cross product t = z X n.

duffymo
  • 305,152
  • 44
  • 369
  • 561
  • Thanks for your comment. As I said in question, is resolving the force only option, I meant the same thing i.e. affine transformation. I want to know that whether ABAQUS provides any way to apply force at angle according to nodal coordinate system. I know that in ANSYS, one could apply force in nodal coordinates. – user3519733 May 06 '14 at 22:18
  • 1
    Usually it's more convenient to use a traction loading (aka pressure) which is normal to the surface. Let ABAQUS do the transformation for you. If you have a spherical shell with a pressure loading on the outside, you wouldn't apply the load with individual forces on nodes. You'd apply a uniform pressure on the surface. – duffymo May 06 '14 at 22:44
  • You are right. But if I have many concentrated forces at angles, then resolving them each along global coordinates will be tedious. So I was searching for some way to apply force at some angle with respect to global coordinates. – user3519733 May 07 '14 at 11:41
  • 1
    My advice is to write code to preprocess your stuff. That's what I usually did when I did FEA for a living and was faced with tedious stuff like this. Write it once, use it forever. As far as I know there is no easy way. Get a shovel and start digging. – duffymo May 07 '14 at 11:47
0

Concentrated forces are applied in the nodal coordinate system. You can use a TRANSFORM on the nodes. For example, to apply a radial load away from the Z axis (lifted from http://www-h.eng.cam.ac.uk/help/programs/fe/abaqus/faq68/abaqusf7.html)

*TRANSFORM, TYPE=C, NSET=CID1
          0.,          0.,          0.,          0.,          0.,          1.
**
*NSET, NSET=CID1
       1,       2,       3,       4,       5
**
**
** radial force
**
*CLOAD, OP=NEW
       1, 1,          1.
       2, 1,          1.
       3, 1,          1.
       4, 1,          1.
       5, 1,          1.

In general though, you'll still need vector components to define the rotated coordinate system for *TRANSFORM but if your angles are uniform in a cylindrical or spherical coordinate system or many nodes have the same angle but different loads, then this will save a lot of tediousness.

user1318499
  • 1,327
  • 11
  • 33