Contacts and constraints in rotating assembly analysis

[anderspilegaard]

Hi,
I have this assembly, where a motor in the middle rotates 10 degrees about the x-axis clockwise and therefore rotates the "fins" (The pin on the pushrod can slide in and out). I would like to find the contact forces between the parts. Right now it is run as a "linear static" until I get it to show results, then it will be made as quasi-static analysis.  The only force counteracting is the friction between all the contact points. I have set all these points as seperation contacts with a coefficient of friciton. 
I have constrained the backside of the brackets in all directions. And the face of the "motor" in the middle is constrained so it can only rotate about the X-axis. And the faces of the "pushrod" where they connect to the motor threads are constrained in the z-direction and rotation about y- and z-axis.
(Coordinate system is seen on image #3 by the way)
Now to the problem:

These are the errors I get when running the simulation, and the results show 0 stresses/displacement:

[John_Holtz]

Hi @anderspilegaard . Welcome to the Inventor Nastran forum.

There are no errors; the list you show indicates that are all warnings. Warnings do not stop the analysis.

Based on your description, you have the following problems.

1. You cannot apply a rotation to a solid. A rotation would require transmitting a moment to a node, and solid elements do not transmit moments through the nodes. You need to apply a rigid body connector in the hole. Then apply the rotation load (and rotation constraint) at the center of the rigid connector. The rotation creates a moment at the center of the connector, and the connector transmits forces to the nodes on the solid. Then the solid "rotates".
2. Friction is not supported in a linear analysis. You may be able to get stresses and displacement, but the results are based on 0 friction.

Let us know how the Explicit Quasi-static analysis goes. (Or maybe start with an Explicit Dynamics analysis to get the analysis to run, then switch to Quasi-static to make it less dynamic.)

John

[anderspilegaard]

Hi,

Thank you. I will run it as quasi-static.
I added the rigid body connector, and applied the rotation and constrait to it. 

I don't know which rigid body type to use; rigid or interpolation. When using interpolation I get this fatal error (X7058): 

When using the rigid body type the simulation ends almost immediately:

[John_Holtz]

Hi @anderspilegaard . Sorry, I was not thinking clearly about using the explicit analysis. It behaves differently than the linear static analysis in regards to enforced motion and the rigid connectors.

I think the window is not wide enough to show the complete error message, but it is probably in a foreign language (the language of Nastran Explicit) which does not translate to engineering. 😁 Please try the following:

1. Use a rigid body connector. The assumption is the motor is more rigid and your model, so using a rigid connector is fine. (Also, you do not have a mass at the center of an interpolation connector, so no need to try that.)
2. The constraint at the center of the rigid connector should constrain all directions except for Rx. That direction is controlled by the enforced motion. (Restraining the other directions says the motor is not moving.) For the explicit analysis types, you do not want a constraint in the same direction as the enforced motion. For all other analysis types, you do want a constraint in the same direction as the enforced motion (because the enforced motion moves the constraint, and the constraint moves the model).

If you still have some type of error, feel free to create a pack and go using these instructions, and attach the zip file to the forum. What files to provide when the model is needed - Autodesk Community

Now that I think about it, have you tried the Inventor Dynamic Simulation? If the goal is to get the contact forces, a simple kinematic analysis would be much faster. Something to think about.

John

[anderspilegaard]

Thanks for the clarification. I had already used a constraint excluding only Rx, but it still did not work. 
You are right about the dynamic simulation - I had not thought about that. I think it will get the job done. So I will try this before looking at the errors from the explicit simulation. 
I'll post an update about it when I have tried it. 
Thank you.