Linear static analysis with cable connector between two components

[Anonymous]

I am trying to run a cable between holes in two parts, fix one surface of one part and apply a normal load on one surface of the other part. I am basically trying to see how the cable responds to tension. I am getting a singularity error and I believe it is due to lack of constraints.

I would greatly appreciate any suggestions as to how I can find a solution to my problem without over constraining my setup. I am unable to get rid of the error unless I have at least one edge/surface of the "loaded" part fully constrained.

Thank you!

[John_Holtz]

Hi @Anonymous 

You have a number of problems in your model:

1. Cable elements are not supported in a linear static analysis. (That is what the Warning T2301 is trying to indicate.) For a linear static stress analysis, you should use a rod connector.
2. The cable/rod connector stretches between two work points, but otherwise it is not connected to either block in the analysis. You need to decide how you want to connect the blocks and cable/rod and then include that in the analysis. In other words, do you want it connected to a single point in each block? (Use a mesh control at the workpoint to create a node on the block that corresponds to the work point that corresponds to the end of the cable/rod.) Do you want to add a rigid connector inside each hole in the blocks and connect the cable/rod between them? Something else?
3. The cable/rod only provides a resistance (a stiffness) in the axial direction. In your model, that would be equivalent to a constraint in the X direction. You need to constraint the "free" block to prevent translation in Y and Z, and rotation about X, Y, and Z. You could restrain the face with the load in Y and Z translation (or the face on the opposite end of the block). That would fix Ty, Tz, and Rx. The block would still be free to rotate about the Y and Z axes (passing through the connection point between the block and cable/rod), so add a Tz constraint to one corner of the block (not on the face with the TyTz constraint!) to prevent rotation about Y. Add a Ty constraint to one corner to prevent rotation about the Z axis. Check the reaction force after the analysis completes to confirm that the reaction is insignificant. (That is, the dummy constraints are just to stabilize the model; they are not restricting the motion.)

The answer to your question "how does the cable respond to tension" is this. The cable/rod responds to tension the same as any slender tension element. The displacement = force*length/modulus of elasticity/cross sectional area. The force in the cable/rod is equal to the applied load (because it all goes through the cable/rod), and everything else is known from the input and the geometry.

[Anonymous]

Hi John,

Thank you so much for your detailed response. I am fairly new to Nastran and I am not a regular FEA user either, so I am having a really hard time understanding most of what you suggested. I hope you wouldn't mind some follow up questions I have to make sure I am going in the right direction.

1) I have switched to Nonlinear Static analysis mode. I am assuming that rods and cables are solved differently in Nastran, so I would like to keep working with a cable to replicate my real world problem.

2) To make it simple and figure out how to work this thing first, I have removed the holes and now I'm just running my cable from one surface of one block to the closest surface of the other block. I have also created nodes on the blocks, at the cable end points.

3) I have added the constraints you pointed out, and I would appreciate it if you could verify them (files attached), because I am still getting the same error.