COMBIN14 and Nodal Coordinate Systems

[MrRogers1987]

I'm using 1D COMBIN14 elements to connect coincident nodes and manually control the stiffness between them for each DOF. The orientation for each spring is based off the nodal coordinate systems of the nodes defining it according to the ANSYS manual. I want to know the forces between these two nodes in a local coordinate system so I aligned the nodal systems with it. When I run my model it behaves as expected, but when I try to recover the forces in the spring elements they are clearly incorrect. In the manual says that if your rotated nodes are not rotated in precisely the same way that force equilibrium won't be maintained. I tried rotating the nodes using both nmodif and nrotat (separate attempts) to ensure that they had "precisely" the same orientations, but it seemed to make no difference. The only time the forces would come out correctly was when there were no rotations applied to the nodes defining the springs.

Is there some other way to define the element orientation that will not inhibit its ability to maintain force equilibrium? Or alternately, is there some way to translate the element forces from the global coordinate system into a local coordinate system after solving?

 

[Drej]

Check your KEYOPTs for the element. The defaults are that the nodes define the element in terms of the coordinate system it operates in. You can use KEYOPT 2 to define/change the coordinate system the element operates in. If the nodes are coincident I'm not sure how the element would behave with the defaults.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[MrRogers1987]

I have 6 individual COMBIN14 elements at each location, for each one I specified a different DOF with keyopt(2). Like I said, the model is functioning properly (i.e. there is an appropriate stiffness in the directions that I defined with the local coordinate system). The issue is when I am post-processing and trying to list the forces in the spring elements - I know what they should be but instead they are all coming out approximately zero. This problem goes away when I don't rotate the nodes at all (i.e. the nodal coordinate systems are the global CS), but then they are not in the directions that I want them (nor are the stiffnesses).

 

[Drej]

If you believe your model is behaving correctly and you only need to "transform" results then consider using the RSYS command wrt a local co-ordinate system.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[MrRogers1987]

Yes I realized that if I specified the CSys for the results then they came out correctly. Odd that the force balance would be thrown off in some coordinate systems but not others. For some reason in global the resultant sum was approximately zero, but when listed in the nodal CSys the resultant was in the 10 kN range as expected. Any ideas why this would be the case? I would've expected it to be able to transfer the load components from the local CSys to global without issues.