Learning Forum

[shamik062]

Hello everyone,

I am trying to do structural dynamic analysis of a vibrating feeder. The feeder comprises of Two main group of parts. 1. The vibrating feeder bowl made up with several plates welded together and 2. The Magnetic Actuator which is imposing motion to vibrating feeder. The feeder and the Actuator is supported on group of Springs only.  Also, the feeder bowl and magnetic actuator are connected by 4 Long Bolts. I have attached an image of the Assembly for better understanding. The imposed motion data is  2.5 mm amplitude with 50 Hz frequency. The direction of the motion is at 19 degrees with the horizontal X axis.

Since I am new in doing dynamic analysis of this kind I am not sure about my analysis. If you can review the analysis it will be highly helpful. I have attached the Ansys Files. 

Thanks in advance.

[Aniket]

Ansys employees are not allowed to download files from the forum but hopefully, the other members can chime in.

-Aniket

Guidelines on the Student Community

How to access ANSYS help links

[peteroznewman]

Shamik,

The Frictionless supports are not what you want. They constrain the model to move on that face relative to ground. Delete Modal 2.

What you want is a translational joint and a joint load that applies the 2.5 mm amplitude of displacement between the magnetic actuator and the feeder bowl.

Then you want to add a Harmonic Response to the end of the Modal and compute the response of the entire structure when that 2.5 mm amplitude has a 50 Hz frequency.

Next time you attach an archive, say what version of ANSYS you are using.

 

[shamik062]

Thanks Peter for your reply. I am working on Ansys 2019R3. I used Frictionless support to guide the Feeder-Bowl to move only in that direction and check the corresponding natural frequencies. 

But I do not understand how to apply Transnational joint or Joint Load. If you can show me the steps that will be highly helpful.

Thanks again for your reply.

 

[peteroznewman]

Shamik,

I made a small model to test my suggestion above out.  The translational joint is working properly, I can see the correct motion in the Modal analysis. See Mode 2.

I assumed a Joint load was allowed in Harmonic Response, but it seems that I was wrong.  I can't get a Joint - Displacement load to be accepted in the Harmonic Response in Mechanical. It's not permitted in either Full Harmonic or MSUP Harmonic. 
Maybe someone from ANSYS will comment.

What I could do was put two Force loads that pointed in opposite directions. These are going to act like the force coming out of the magnetic shaker in that they will push and pull the two pieces along the axis of the translation joint.

Here is the Frequency Response of one vertex in the X direction.

I hope the attached model gives you some ideas for your larger model.

Regards,
Peter

[shamik062]

Thank you so much peter for your help. I have looked into your model. Before applying the joint connection to my model I have few questions.

1. I have used 4 beams (by line body construction) to idealize the long bolts which connects vibrating feeder bowl and the magnetic actuator. So what is the purpose of using transnational joints between feeder bowl and the actuator?

2. Does it constrain the feeder to move in a specified direction?

3. Also if I simultaneously use beams and joint between feeder and actuator will that over constrain the system?

4. Another thing I noticed in your model that you have created remotes points and then attached the springs with that points. I did not used the remote points. Instead I have created only the co-ordinates for the springs by geometry selection and then used the origin to attach the springs. Now what is the difference between these two situation?

Thanks again for you help peter. I will apply your method in model and check my  results.

[peteroznewman]

1. Beams don't allow one body to translate freely along the length of the beam, that is what a translational joint allows.

2. Translational joint provides exactly 1 DOF between the two ends, axial motion along the line connecting the two ends. The two ends define the axis of freedom, which can move about in space following the two ends.  

3. If you add a beam, it will constrain the axial freedom that the translational joint provided.

4. To connect 3 springs to the same edge of the model, create one remote point on that edge, then connect 3 springs to that one remote point.  That is the correct way to build the model.  If you connect 3 springs to the same edge, you will get a Warning about overconstraint of MPC, etc.

[shamik062]

Sorry for late reply as I was caught up with some other jobs. I tried your method in Modal Solution. It is working properly. My project was basically a design assessment where some crack originated and  propagated at the weld location between feeder plate and base of the vibrating feeder. So my initial thought was that the structure is in resonating condition and there might be a stress amplitude. But even after applying your method the first 6 natural frequency is no where near the excitation frequency. So I did not perform a subsequent harmonic analysis. Instead I did a static analysis with inertia relief and calculated the fatigue life at weld location based on Hot Spot Method and the results indicates that the plates of the feeder at weld location has finite life.

If you have any thought on my analysis methodology kindly share with me and thanks again for your help.