we want to use SKF 6302 near rotor disk and 6304 bearing on the other end.
We modified the model based on your suggestion to apply max torque of 20Nm and RPM of 9000 to 9500 but it runs for ages. Have we done anything wrong?.
It might be hard to get it to converge with frictional contact between all 3 parts and applied moment. You may have to replace the moment with a prescribed rotation boundary condition on the reference point (you will have to estimate the angle of rotation and then you can check the reaction moment to adjust it if needed). However, keep in mind that contact between all parts is necessary only if you have to account for the fact they can slide on each other during the operation. If any of them are actually “glued” together, you can use tie constraints or merge the parts instead.
Thanks a bunch ur right we need to use TIE. I think I made a mistake as the parts will be glued.
I have one last Q. How to check the gyroscopic effect of the rotor so that we can take this as an input for bearing life impact.
What is that we need to change in the model ?.
To do that you could add two steps to your existing static step with centrifugal load - frequency and complex frequency (available in PrePoMax 1.4.0). The static step needs Nlgeom enabled and the two frequency steps should have storage and perturbation parameters enabled.
Check this thread for more details and some examples: Modal Analysis of Centrifugal Compressor Impeller
It’s just a warning, normal if you have tie constraints with slave node adjustment enabled which results in a slightly different mesh than defined initially.
After running all the scenarios we are little bit confussed now on the actual forces we need to take as input for the bearings from your software at two locations please ( scenario 1: Max 20Nm torque in the rotor and scenario 2: maximum rpm of the rotor shaft 10000). Can you please help us understand what should be the forces we need to consider as input based on the above models we have created?.
Did you request the RF history output for the boundary condition (bearing) region as explained here ? This should give you forces in each direction.
We created a simple model as below by taking total mass of the rotor to get a clear understanding on the forces to consider as input. Is the model correct and are values of history output correct pls please?.
It is definitely a good idea to build a simplified model in such cases. However, in that file, boundary conditions are applied to faces:
You should apply them to reference points of rigid body constraints instead:
Then you will get the reaction forces from the directions where you set the BC to 0.
RF1 - force in the X direction
RF2 - force in the Y direction
RF3 - force in the Z direction
RM1 - moment about the X direction
RM2 - moment about the Y direction
RM3 - moment about the Z direction
The rest should be clear. You have reference point 1 and 2 so there are 12 outputs in total.
In our output for Reference Point -1 We have 361499[N] and for RF2 we have 361499[N].
Are you saying we have force in KN ?. Is this correct pls.
Those aren’t the forces, those are the REF and ROT NODE numbers. Forces (and moments) are in the rows below - next to 1.
Thanks. We will try with the actual rotor , include manufacturing tolerances ( eccentricity, etc and tolerance). As it has to be practical.
I appreciate all ur help.
Hi,
We have a question please.
Till now we have been running analysis on the motor torque and rpm effect. Well now if the motor is turned off( power is off) and the rotor is acting like a fly wheel we want to check the effects on the rotor( motor will be in generator mode). we built the below model i.e. to check if we rotate the rotor shaft at 10000 rpm what will be the effect on the overall rotor but it seems we are doing something wrong. Can you please check and let us know your feedback.
When you apply BCs via rigid body constraints, you should also fix the rotations of their reference nodes (UR1, UR2, UR3) to avoid rigid body motions. Also, centrifugal force load is applied only to one part. And finally, there are errors due to overconstraints - apparently, some tie constraints overlap. Either check their definitions or just use compounding on the parts instead - will be easier.