Suppose that I have a long shaft modeled with 3D elements. There are two bearings at the end of each shaft and would like to see the effects of bearing stiffnes on shaft vibration modes.
What can be the best modeling approach for ball bearings in Simcenter, CBUSH elements ?
Looking forward to you valuable comments.
Using springs (i.e. CBUSH) for bearings is a widely used approach. If you aren't modeling the structure beyond the bearings, then you could use node to ground CBUSH elements. These are 1 node elements that connect to your structure, then to ground as if it is a 2 node element with one of the nodes fixed.
This is a study we could do in Simcenter Motion using flexible bodies. We can mount the shaft on bushings that you can define either a linear or varible stiffness and damping. We can then spin the shaft at a range of RPM's and study the shaft vibrations at each RPM or bearing stiffness.
I agree with the recommendation to use CBUSH. Since CBUSH is node-to-node (or node-to-ground) you would need to create connect nodes on your 3D shaft model. I would recommend that you use RBE3 element to connect a group of nodes on your shaft to a centerline node (that is not part of a shaft element). Then you can connect CBUSH to the RBE3 node.
Moment stiffness is often the most important to get right. Generally the translational stiffness of bearings is high relative to the shaft stiffness lateral stiffness. In that case it almost behaves rigidly. But bearings also transmit moment stiffness by virtue of having a length. This stiffness is often on the order of shaft bending stiffness so will have a signficant effect on the response. You may be able to find moment stiffnesses and use those as part of the CBUSH. Or you can create several CBUSH elements that span the lenght of the bearing and give them traslational stiffness only. This will also result in bending stiffness.
If you have no idea what to use for bushing stiffness values, you could make a detailed break-out model of your shaft and the bearings modeled explicilty with 3D elements. make contact connnections between the shaft and bearings. Apply a vertical (or lateral) load to the shaft representing the weight that goes into the bearing. This will establish your reference condition. Then apply another load that may be twice the load of the first. You can use the delta load and delta displacement to compute a stiffness for the CBUSH. You can do similar to get a moment stiffness.
Thank you for your explanation.
What about for the other side of the bearing (supoort structure or housing)? Should we also create an independent node and connect with RBE3s to the support structure, then connect the two nodes with CBUSH ?
Do you have any sample models to show the usage of CBUSH as bearings ?
I am trying to do a similar problem. I created a Rb3 for the support structure and an Rb3 for the shaft surface. Then i joined the two dependent nodes of those two Rb3 using a CBush element, but the Nastran gives errors. Like "the bush element has infinitesimal length and NOGO encountered in SUBDMAP", can you hep with these errors. ALso I am unable to downlaod your files, the downloaded files has 0 Kb size. Can you email me your NX files at "firstname.lastname@example.org".
I don't recall the files I sent previously. But the error you are getting now seems to indicate that you are using a CBUSH element and the 2 nodes at the ends of the CBUSH are coincident. When they are coincident like this, you need to specify a coordinate system to define the orientaion. The error message seems to indicate that perhaps you do not have the coordinate system defined. In the Nastran input file, it is field 9 on the CBUSH card. I suggest you check that first and correct as needed.
Thanks for replying.
I have few questions if you can answer them,
1. for CSYS: I have to go to mesh associated data and enable CSYS to override, I gave it absolute coordinate system, does this coordinate system define the orientation of the spring element or does it define the coordinate system used to define the stiffness values along six dof.
2. How can one measure or come up with the numbers for the six stiffness values?
3. Instead of using Cbush grounded, I used cbush 1d element. I defined a RB3 from shaft outer surface which is in contact with bearing and other RB3 from support inner face that is in contact with the inner bearing face. Then I connected both RB3 centre node using CBUSH element. Is it a correct representation of bearing.I could not use CBUSH grounded as for some reason it was not selecting the RB3 node for that element.
I have attached a copy of how the shaft and outer support looks like, since Cbush is infinite small it is not visible.