Ansys Workbench - Beam 188 and Link 180 element - together?

[SukiLeinen]

Using : Ansys Workbench 16 Educational
I want to build simple frame and simulate stress state and deformation when that frame is lifted.

I have constructed my geometry in Design Modeler using line body's.
My lifting cable has circular cross section with diameter of 10 mm.
My frame has square hollow section 40x40x2 mm.
After modeling everything is converted to one part with Form new part command.

In Model setup I have used line pressure on central beam and displacement (x=0,y=0,z=0) for support on top where 4 cables meet.

I have added command object to 4 line body that are representing cables:

ET,matid,LINK180
KEYOPT,matid,3,1
SECTYPE,matid,LINK
SECDATA,78.6

When I run my analsys I get error (no result):

There are 112 small equation solver pivot terms

What am I doing wrong. How to use Link 180 and Beam 188 element together and simulate stress when frame is in lifted state - when it is lifted in air (cable - tension only in cable)

Can someone explain me (in Ansys Workbench) how to approach this problem.

This problem is for educational purposes.

 

[SukiLeinen]

Any help :) ?

 

[Mech_Engineer]

For a start, can you give us a picture showing your current geometry, and the boundary conditions you've applied to it? A picture is worth 1000 words!

 

[Julsmo]

hi all,
I am getting a similar error and am trying to model cables and beams as well.I attached a picture of my geometrie. the frame constrained in all dof and the inner lines are cables defined as link elements with combin14 elements at two coincident nodes between each link element. the combin elements are element number 1 to 82 for what i checked and get a rotational stiffness around the Y axis
*** ERROR *** SUPPRESSED MESSAGE CP = 4.297 TIME= 09:12:48
A large negative pivot value ( -3.36894895 ) has been encountered in
the global assembled matrix at the UY degree of freedom of node 1510.
This may be caused by a bad temperature-dependent material property
used in the model.

*** ERROR *** SUPPRESSED MESSAGE CP = 4.297 TIME= 09:12:48
There are 102 small equation solver pivot terms (e.g., at the UY degree
of freedom of node 2175). Please check for an insufficiently
constrained model.
those are the main error messages i assume. why is that and what does it mean? could it be possible, that this happened because I am creating more than one element for each line (that's supposed to be one link element)?

 

[Mech_Engineer]

The solver appears to be complaining that the model is under-constrained. Are you sure all of your nodes are connected in the middle of the model?

 

[Julsmo]

thanks for the fast reply!
I believe so. I tried to assign the beam section and properties to all lines (not only the frame) and that works fine. No error message with calculating. If I try to model the inner lines as link elements and use the same boundary conditions and all, i get that error. So my assumption would be a problem with defining or meshing the link element.

 

[Mech_Engineer]

Link elements are only able to model axial tension/compression. Shouldn't you be using Beam elements to take into account bending moments as well?

 

[Julsmo]

I plan to make different models. one also with calculation the moment of inertia of cables. but in my understanding it would also be correct to model a cable with multiple link elements since a cable itself can take nonaxial loads only after being deformed (slag being the mirrored bending moment). In that case I am getting the stiffness by adding pretension to the cables and also by modeling the intersecting points with a rotational spring.Just need the link elements to work nor nodal load perpendicular to the plane of the net. would be really greatful for any suggestions?

 

[Mech_Engineer]

Why don't you try with beam elements first and see if it works, and we can work from there. I'll bet the link element mesh is giving you problems because of the extra degrees of freedom and each intermediate node in your geometry (since link elements cannot support a moment load at their ends).

 

[Julsmo]

I already tried with beam elements for all elements to check the geometry and see if there is any double nodes etc. That works. Sorry guess I forgot to write that.

 

[Julsmo]

I only have a nodal force at the end node of a link element though. That shouldn't be the deal. I believe it's something about the meshing of the link element. But I am not an expert with ansys...

 

[Mech_Engineer]

I only have a nodal force at the end node of a link element though. That shouldn't be the deal. I believe it's something about the meshing of the link element. But I am not an expert with ansys...

The important thing to keep in mind is a Link element can only register a vector force because each node has only 3 degrees of freedom (Ux, Uy, and Uz). Beam elements on the other hand have 6 degrees of freedom at each node (UX, UY, UZ, ROTX, ROTY, ROTZ), which allows the calculation of both force and moment at each node. In the case of a mesh with beam elements, the shared node between two beam elements acts as a boundary condition because the moments have to balance.

My guess is as I said before, your mesh is under-constrained when you use link elements because they do not have moment loads between connected elements. From what you've described, your geometry doesn't seem like it will work with Link elements without more constraints.

See here: LINK180 Element Description, Beam 188 Element Description