How do I contrain an axle

[Anonymous]

I am trying to calculate the stress in four beams which are connected by a couple of axles. The beams are arranged in a scissor formation, as seen in the picture below.

The left corner is constrained in every direction but Ry (so it can rotate around the axle). This is done by making a rigid body from the centre of the hole to the outside of the hole (all the dependent entities are checked)  . At the same centre, a constrain is placed where all dependent entities but the Ry are checked.

The right bottom corner is constrained in the same way, the only difference is that this corner can also move in the X-direction. So Tx is also unchecked.

The top two corners both have a bearing load on the face of the hole, as shown in the picture below:

The real problem occures at the connections between the four beams. At the centres of the beams (where they connect), I placed a Beam element from 10 mm long (the beam itself it 200 mm). From this beam element, i made a Rigid body to the beam it was placed on. On this beam, the rigid body was fully constrained. From this same beam element, i made a rigid body to the beam next to it. This beam was fully constrained, but in the Y rotation.

The mesh is set to 20 mm and all the contacts are made automaticly.

When I run the simulation, the stress level around the holes are unrealistically high. Where the rest of the beam seems normal. How can i make the constrain so that I will see normal stress levels around the axle points? 

[John_Holtz]

Nice description @Anonymous 

There is just a couple of minor things that you need to do differently.

1. Just for your information, the "degrees of freedom" check boxes on the rigid connectors are not constraints. They indicate what loads (forces and moments) are transmitted from the rigid connector to the model. Since the connectors are attached to solid elements, and since solid elements only transmit forces, checking TxTyTz is the same as TxTyTzRxRyRz and TxTyTzRxRz. In other words, the R checkboxes do not make a difference because moments cannot be transferred into a solid element. (In your original post where you described the rigid connectors at the linkage between the two scissor sections, you referred to the check boxes for the dependent entities as "constraints".)
2. ALL LOADS are transmitted to the center point of the rigid connector REGARDLESS of what degrees of freedom are checked for the dependent entities. This is where the analysis is not behaving like you wanted. Essentially, the pins/shafts between the scissor sections are behaving as if they are frozen/welded to both beams of the scissor, so they are not allowing the intended rotation. What you need to do is add an end release to ONE END of the beam element (at each joint) to free the Rx rotation. So one end of the beam element is welded to the scissor; this prevents the beam element from rotating like a pin held by two bearings. The opposite end of the beam is free in the torsion direction (Rx), so it will not transmit a torque to the adjoining scissor. Therefore, it will behave like a pin in a linkage.
3. I cannot determine from your images what you selected for the rigid connectors. If you only selected the two outside edges of the hole through the scissor, this would partially explain why the stress is high around the edge of the hole. It might go down after your add the end release to the beam, but it still might concentrate the "reaction force" over a small area. It might be better to select the face that is the I.D. of the hole so that the load from the pin/shaft is distributed over the "contact" area between the pin and scissor.

If you are doing a linear static analysis, that is all you need to do. If this is a nonlinear, large displacement analysis, then you also need to do something so that the rigid connectors follow the large deformation theory required for large displacements. See this article for details: How to create a pin connection between linkages in Inventor Nastran.