I am looking for a kinematic coupling constraint between a reference node and a cylindrical surface in ANSYS Workbench. I am unable to find it. Let me know how can we apply the constraint between a node and a surface.
You ask about a kinematic coupling between a reference node and other nodes. Open the ANSYS Help system. Navigate to the Mechanical APDL section and then into Chapter 10: Multipoint Constraints and Assemblies. In there you will see there is an APDL command CP for Coupling, a CE command for Constraint Equations, an RBE3 command that distributes forces from a master node to a set of slave nodes. In these commands, specific Degrees of Freedom can be coupled, and these are defined in the nodal coordinate system.
If you want to constrain three nodes to ground in a pattern that allows free radial expansion, that is easily achieved by creating a Cylindrical Coordinate System. In that system X=Radial, Y=Theta, Z=Z. Put the origin of the Cylindrical coordinate system at the center of the cylindrical surface, and align the Z axis with the axis of the cylinder. If you pick three nodes around the circle, you can constrain Y=0 and Z=0 and leave X=Free. Now a Static Structural model will solve without pivot errors. This can be done in Workbench without using any APDL commands.
I want to apply a coupling constraint between a reference node and a cylindrical surface so that I can apply a force at the centre of the cylinder on the reference node. I m working in ANSYS workbench using static structural. Also, the cylinder is a part of a huge assembly.
In Workbench, simply apply a Remote Force and scope it to the cylindrical face. A remote point will be created at the center of the face. In the details of the Remote Force, set the Behavior to Deformable. That will distribute the force to all the nodes on the face without adding any stiffness.
Remote force does not work with Cyclic Symmetry. I got an error.
You have a choice: abandon cyclic symmetry and stay in Workbench, or keep cyclic symmetry and dive into APDL commands to achieve what you want with cyclic symmetry. Good luck!
If I abandon cyclic symmetry, then computation time increases. It also gives me an error of the elapsed time exceeded the CPU time by an excessive margin.
I have taken a sector of the geometry (shown below) in order to reduce time. I want to apply a vertical loading at the centre as shown. Kindly guide me on how to do so.
Abandon cyclic symmetry because the compression of the spokes on the bottom and the tension of the spokes on the top are not what I understand to be cyclically symmetric.
Also, the figure shows a Rigid hub. In that case, the Remote Displacement would be Behavior = Rigid, not Deformable.
I suggest you convert this to a Plane Strain 2D model to reduce the computation time.
The message that the elapsed time exceeded the CPU time by an excessive margin is not an error, it is just informing you that your computing hardware is not optimal. If you had more RAM and faster storage (like a SSD), then the elapsed time would be close to the CPU time.
If I convert into a 2D model, then how would I get the contact pressure with the ground?
A 2D plane strain model can have contact pressure with the ground but it will have no end effects. The pressure will be in terms of a unit depth.
2D plane strain model works if the geometry in the z axis is same throughout. In my case, geometry in the Z axis varies.
To reduce the long computation time of a fully solid element mesh in 3D, convert the thin walled deformable spokes into midsurface sheet bodies and mesh them with shell elements. Or just get used to solve times that are tens of hours long.
I have attached the picture of the geometry. How can I reduce the computation time?
Isn't that lattice solid? That is not helping, in fact it is worse than the original image you showed.
I suggested you replace solid spokes with surface bodies by using the Midsurface button.
Yes Peter. I am working with lattice structures.
If you start with a honeycomb structure like you showed initially, you can convert that to a sheet body configuration instead of a solid body.
That is how you can reduce computation time. Do you know how to do that? If not, watch a SpaceClaim tutorial on Midsurface feature.
A solid element mesh on that geometry will overwhelm your computer.
I recommend you study ANSYS Material Designer and generate an RVE to replace that geometry with equivalent elements.
I have nothing else to add to this discussion. Good luck.
I studied the ANSYS Material Designer and RVE generation but I am unable to understand how it is applied to the lattice model I am working on?
I haven't studied RVE generation. Maybe someone else can help. I have nothing else to add.
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.