How do you increase the number of degrees of freedom of a component? I keep getting an error in a rotation I am trying to do. The error says that the components selected do not have enough degrees of freedom.
A rigid body in 3D space has exactly six degrees of freedom. Different boundary conditions or joints take away different degrees of freedom. Are you doing Rigid Dynamics or Static Structural or some other analysis?
Please reply with a screen snapshot or some kind of illustration of the component, the rotation you are trying to do and the supports that are currently defined on the component.
Thank you for your response. I am doing a steady/static analysis in aim.
The supports are highlighted:
All 4 contacts like this are "No separation" so that that large cylinder can roll on the 4 smaller cylinders.
I am trying to make the below selection rotate about its center.
Here is the error
No Separation contact with the four small rollers take away four degrees of freedom from the large roller.
To do a static analysis, you actually need to take away two more degrees of freedom: rotation about the cylinder axis and translation along the cylindrical axis, otherwise there is no solution to the matrix inversion (except when weak springs are used).
A no separation contact of a small cylindrical roller on a large cylindrical surface prevents the cylindrical surface from tilting up on one edge when the center of the tube between the span sags under gravity, and the prevention of a lift-off creates an artificial stiffness.
I would change the four small rollers to be frictional contact with the two large rings. That way the large ring can tilt a little if it wants to due to bending of the center of the tube. You can put a revolute joint on all four small rollers. Then on one of the four small rollers, you can put a joint load on the revolute, which would be a rotational displacement. You can ramp that displacement up in angle and friction will cause the large tube to rotate on the four small rollers. The friction also prevents the translation along the axis. Then you can get a series of static equilibrium at different angles of the large drum.
Thanks for your help on this! Your advice makes sense. I changed the roller contacts to frictional but revolute joint does not appear under joints in aim. My options for joint behavior are: Fixed, Hinge, Slot, Cylindrical, Universal, Spherical, Planar, and general. Should I select Hinge?
Also I Have been getting some odd displacement results. I "turned on gravity" by creating an inertial load on in the negative y direction but I am get displacements in the positive y and the side of the barrel are being crumpled in. I this the correct way to turn gravity on in Aim? I'll send a picture in a bit.
Yes, Hinge = Revolute.
Yes, gravity is an inertial load with a specific acceleration of 9.8 m/s/s but in Mechanical (and I assume AIM), you accelerate upward in the positive Y direction to apply a downward (negative Y) force on a mass.
That is very helpful to know. I really appreciate you taking the time to help me.
I want to static structural analysis on ECAP system but i am not able to give a system proper dof can some help me to do it or guide me
i am sending screen shot
this is my system i want work piece to flow through the tube i applied pressure on the top face but i am not able to define dof conditions
Waqas, Open a new discussion and explain your problem in detail using pictures as Roy did in this discussion.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.