APDL use of Combin7 elements 1

[SafetyFactorOf1]

Hello everybody,

I've just started a new project somewhat outside of my usual work description and was wondering if you guys could provide some guidance for me, as the APDL command reference isn't quite answering my questions. I am essentially looking to build a parametric model of a tubular steel structure, subject to specific forces through it's range of motion. What I would like to do is model the hinge assembly in the large scale beam model to get an overall idea of compliance for various tube sizes and configurations, and upon satisfactory results, design mountings, hinges and connections through "hand" calcs.

My questions are:
-My current plan is to lay out keypoints and lines, meshing as beam189 elements, and use combin7 elements to model the rotational joints. Am I correct in this approach, or is there a more appropriate method? This method would lead to two keypoints at the same point in space, allowing me to mesh two components separately. Thoughts?

-I am a bit concerned regarding the use of combin7 elements, and would like some input. The hinges actuate at an inconsistent with global coordinates. I can work out the angles, but I am concerned that imprecision in the resulting calculations may artificially stiffen the joint/structure resulting in incorrect results. What is the tolerance for these sorts of things in ansys, and would I perhaps be better defining a local coordinate system at the joint? My understanding of combin7 is that it requires 3 nodes, the two nodes from the two elements to be connected and another node to orient it. What would happen if I placed a node in space to orient the actuation of the joint, but did not connect it to anything? Would this be problematic?

-Finally, since I am using keypoints to "outline" the structure, these joints will occur in the model at two specific keypoints, occupying the same space, as described above. I am a little confused in the scripting here and my first thought is to use a piece of code to essentially select the two nodes occurring at the single location by referencing the two respective keypoints in order to give me two variables representing these selected nodes. From here, I would use these two variables to define two of the three nodes for the joints. I am still left with the issue stated above regarding orientation, but I'll hopefully figure that out. I found a piece of code elsewhere on the forum, which I suspect may be in the right direction...

"keypoint_nr=#####
node_nr=node(kx(keypoint_nr),ky(keypoint_nr),kz(keypoint_nr))"

Thoughts on this method?



I really appreciate you guys taking the time to help me out and either let me know I'm on the right track, or full of you-know-what

Jim

 

[meshparts]

Hello Jim,

Combin7 is an undocumented element in Ansys 14.5. What version are you using? There is a new element (MPC184 Revolute Joint) which has similar capabilities. On the other hand, these elements (combin7 and mpc184) are pretty complex in use with lots of options and properties including nonlinear behavior. Do you really need that complexity? If not a more simple (documented) element is combin14.

You get it right: you need two coincident nodes and define the joint element in-between.

Most discrete elements in Ansys work in the nodal coordinate system. So if the joints acting direction is not parallel to the global coordinate system, you just have to rotate the nodal coordinate system as you wish (see NROTAT command). The third node of the combin7 element is optional. Default is the nodal Z direction of the nodes. I think is more simple an elegant to rotate the nodes instead of defining the third node.

Defining the joint between two coincident keypoints is simple and there are different ways to do that. Here is my favorite solution:

! select keypoints
Kp1=… ! keypoint number 1
Kp2=… ! keypoint number 2
Ksel,s,,,kp1
Ksel,a,,,kp2
! Select nodes on these keypoints
Nslk
! Get node numbers
Nd1=ndnext(0)
Nd2=ndnext(Nd1)
! Define joint element
Type,…
Real,…
Secnum,…
E,nd1,nd2

Best regards,
Alex


MESHPARTS
Tuning Your Simulation

http://www.meshparts.de

 

[SafetyFactorOf1]

Alex,

Thank you very much for your help! I will give this a shot when we re-open on Monday!

I'm using version 13.0

-Jim