Hi together,
I am currently working on a cylindrical segment model with shell elements. Now I want to apply a moment about the global z axis on a set of nodes (this axis is the rotational axis of the cylindrical segment).
My idea is to create a node in the z axis and then to apply the moment on this node but i dont know how to couple this node with my set of nodes from the cylindrical segment.
I am using LS Dyna within Ansys Workbench but manually editing the input.k with keywords is no problem for me.
greets
Hi @hunterx777,
I believe you can do what you have illustrated pretty easily. First, create a *set_node of the nodes that you want to constrain to the single node. Then you might want to apply a constraint to that single node so that it can only rotate about the z axis. You can do this with *Boundary_spc_node and make all the constraints 1 except for DOFRZ.
Now you want to apply the moment to the node using *Load_node_point and set your DOF to 7 and then create your moment curve and reference in the LCID.
Let me know if this works for you.
Thanks for your answer. I tried this and experienced an error that says I have a massless node (my created "external point"). With *ELEMENT_MASS I put a little mass on it and the error went away. As I look in my results there is no deformation of my model so it didnt work. As you described, I think the linking/coupling is missing between the one node in the z-axis and the uppers nodes ("oben") in *NODE_SET.
My "code":
$
*NODE
95 0.00000000 0.00000000 600.00000000
*ELEMENT_MASS
$# eid nid mass pid
46 95 0.01 0
*SET_NODE_LIST
89
1 2 12 14 16
*BOUNDARY_SPC_NODE
$# nid cid dofx dofy dofz dofrx dofry dofrz
95 158 1 1 1 1 1 0
*LOAD_NODE_POINT
$# nid dof lcid sf cid m1 m2 m3
95 7 99 1.0 158 0 0 0
I tried another way with the use of a rigid body. First I applied an "external displacement" on my "external point" about a rotation about the global z-axis e.g. 5 degrees. The "external point" is coupled with the nodes of the set "oben". All done within the Workbench GUI. My results are displaying a rotation about the global z-axis just like I want but with applying of a moment instead of a defined rotation. Then I had a look at my input.k to know what kewords and input data was used for this.
For rotation *BOUNDARY_PRESCRIBED_MOTION_RIGID was used, I replaced this keyword with *LOAD_RIGID_BODY
My "code":
*NODE
95 0.00000000 0.00000000 600.00000000
*SET_NODE_LIST
89
95 1 2 12 14 16
*CONSTRAINED_NODAL_RIGID_BODY_INERTIA
$ pid cid nsid pnode iprt drflag rrflag unused1
2 158 89 0 0 0 0
$ xc yc zc tm ircs nodeid
0.0 0.0 0.0 0.000471 0 95
$ ixx ixy ixz iyy iyz izz
463.2 0.026805 0.0 7.761 0.0 471.0
$ vtx vty vtz vrx vry vrz unused4
0.0 0.0 0.0 0.0 0.0 0.0
*LOAD_RIGID_BODY
$# pid dof lcid sf cid m1 m2 m3
2 7 99 1.0 158 0 0 0
$
The manual says to *LOAD_RIGID_BODY:
The force is applied at the center of mass or a moment is applied around a global axis.
In my results you can see that the moment is applied like in the middle of node set "oben" and not about the global z-axis. I have no idea why this isnt working.
@hunterx777 Nice job solving through this. There are usually quite a few ways to accomplish something in LS-Dyna.
In your *Load_rigid_body, it looks like you have a coordinate system defined (CID). This should act as the coordinate system about where the load is applied. Where is this?
The coordinate system cid=158 is located colinear with the default coordinate system but moved z=+600mm so thats on the same height as the node set "oben".
After I changed drflag=7 ("release 𝑥, 𝑦, and 𝑧 displacement in rigid body local system"), rrflag=7 ("release 𝑥, 𝑦, and 𝑧 rotations in rigid body local system") and cid=21 (21 is the default coordinate system) it is working.
It works only with the flag "+7" and not with "-7" (release displacement and rotation in global system).
The problem now is that I applied a positive moment about the z-axis but the results showing a negative rotation about the z-axis. Thats strange but I can live with that.
