# Need To apply external vibration

• 2.5K Views
• Last Post 02 July 2019
• Topic Is Solved
masud407 posted this 02 April 2018

I would like to apply an external vibration with fixed frequency and amplitude on human body model in ANSYS. How can I do that?

• Liked by
peteroznewman posted this 02 July 2019

Hi jinyan,

Regards,
Peter

jinyan posted this 02 July 2019

Hi

I also doing this project as the master report, I also met the problem about vibration frequency and amplitude, can u help me to solve this please? please contact me with the email jyan16@sheffield.ac.uk or 352904723@qq.com

thank u

jinyan

peteroznewman posted this 05 October 2018

Moved your new question to a new discussion.

peteroznewman posted this 26 September 2018

Hello Masud,

You can get the reaction force at exactly one point due to the applied sinusoidal displacement, that is at the joint.

Every other (any) point is a continuum that has an elastic stiffness and a density. The acceleration acts on the mass causing a force. The force is resisted by the stiffness of the material. The material is deformed by the force. The deformation creates strain in the material. The material modulus defines the stress that stain has created.

I'm not sure what you mean by reaction force at any point. You can plot the acceleration of any point.

Regards,

Peter

masud407 posted this 25 September 2018

Hello Peter,

I was trying to get the reaction force at any point due to applied sinusoidal displacement by using the probe in the solution section. However, it was showing that there is no weak spring to obtain the reaction force. So what should I add to get the reaction force at any point?

Attached Files

peteroznewman posted this 08 September 2018

Hello Masud,

Your second post in this discussion said,

Actually, I want to simulate Whole body vibration (WBV) process in ANSYS. For that, I have to apply fixed frequency and fixed amplitude vibration from the bottom of seated/standing human model. So I want to how can I apply such kind of external vibration?

So put a human model on a seat, but the seat frame is going to be fixed to a translational joint that creates the vibration. You have the cosine function for moving the seat up and down. I don't understand why you want a "hinged support at the other end".

Perhaps you could provide a sketch of the human body on a seat to show where you hope to get to with this simulation.

Regards,

Peter

masud407 posted this 08 September 2018

Hello Peter,

Thanks for your description. Actually, your uploaded file is not working in my ANSYS 15.0 as the version is different. I have managed to run it keeping the Y direction free in the remote displacement section. But I want to provide hinged support at the other end of applying vibration.  I was trying to allow rotation along X/Y/Z direction. Therefore, I was trying to provide rotation in the remote displacement section. Is it the right way to provide the hinged support at the other end?

Yes, my vibration is really low comparing to the structure. Actually, I will try for higher frequency manually or using vibration data (although I don't know how to do it in VibrationData). My target is to draw the difference in mechanical properties (stress, strain, displacement etc.) for the lower vibration range which is mostly used at the lower part of the body.

peteroznewman posted this 07 September 2018

Masud,

You did not seem to understand my previous comment.

You have a translational joint that only allows motion in the global Y direction and you are enforcing an 8 mm cosine motion in the Y direction at that end.

And you also have a remote displacement at the other end of the structure that says zero motion in Y.

Do you understand that these two inputs to the model are in conflict and cannot both be accommodated?

If I change the Remote Displacement and allow the Y displacement to be free, that removes the conflict. Why do you even need a Remote displacement if the translational joint and displacement load has fully defined the rigid body motion of the structure?

The idea is that whatever face is picked for the translational joint, that is the face that is bonded to the shaker table. Everything else is going along for the ride. Hence, there is no need for a Remote Displacement that the other end.

I changed the Joint to attach to the Bone, not the Bone and the Muscle.

I changed the Auto Time Stepping parameters. Now it solves without a problem, but it is not a very interesting result, because an 8 mm displacement in 2 seconds is such low acceleration, that noting is happening.

Attached is an ANSYS 19.1 archive.

Regards,

Peter

Attached Files

• Liked by
masud407 posted this 06 September 2018

Sorry for describing the problem properly. I actually tried to put the displacement at bone only. Still, I am finding the error which says "Solution is unable to converge due to non-linearity". As you said that I am applying displacement of 8mm at one end and 0 mm at another end for t=1 sec. different displacement at the same time at two different ends can be responsible for not getting any solution. But, I just put a cosine function as displacement at one end and leave the other end free as I want to simulate hinged support. So I am not getting any clue to provide the same displacement at t=1 sec. For your convenience, I have attached the file

Attached Files

peteroznewman posted this 06 September 2018

Hello Masud,

When you say

How can I resolve the issue of 8 mm displacement at t=1 sec for the joint displacement?

I don't understand what the issue is that you need to resolve. Do you mean that the solver will not converge? Please clarify.

Regards,

Peter

masud407 posted this 06 September 2018

Hello Peter,

I tried with applying displacement on bone faces and leaving the muscle to just bond to the bone. Still, the solution is unable to converge. Yes, I would like to leave Y axis free in the remote displacement. I just put joint displacement (with sine/cos formula) at one end, but it is showing 8 mm displacement at t=1. How can I resolve the issue of 8 mm displacement at t=1 sec for the joint displacement?

peteroznewman posted this 31 August 2018

Hello Masud,

You have conflicting boundary conditions.  On one end you have zero displacement,

while on the other end you have a Translational joint displacement of 8 mm.

I assume you meant to leave the Y axis free in the Remote Displacement.

You might have better luck with convergence if you just apply displacements to bone faces and leave the muscle to just bond to the bone.

Regards,

Peter

masud407 posted this 31 August 2018

Hello Peter,

I tried to put vibration at one end (joint displacement) and hinge support(using remote displacement) at another end. It seemed like I have done everything okay. However, an error is showing which says "one or two elements have become highly distorted." Can you please tell me where I am making mistake? Thanks.

Attached Files

peteroznewman posted this 20 August 2018

Hello Masud,

See how in my example, the displacement starts at zero?

See how in your equation, the displacement at the start is not zero?

Try changing your equation to this: .004*cos(182*time)-.004

Regards,
Peter

• Liked by
masud407 posted this 20 August 2018

Hello Peter,

I understand your point. I have run the file that you sent me in the last week. However, I tried to put my required amplitude and frequency in my joint displacement function (using cos function). Unfortunately, it is saying that the solution is unable to converge. I have attached the file as well for your convenience (2nd part). What can be the problem? Also, I was facing problem while changing the mesh.

Attached Files

peteroznewman posted this 18 August 2018

Masud,

I'm not surprised that changing the displacement function from cosine to sine creates convergence problems. Take the first derivative of the displacement function to get velocity as a function of time.  The derivative of cosine at t=0 is zero, which gradually increases over time. The derivative of sine at t=0 is not zero. That means the system experiences a sudden impact due to a step change from zero velocity to non-zero velocity in an instant at t=0.  Step changes are never good for convergence.

The only difference adding in gravity will be the sag of the muscle on the bone.

masud407 posted this 17 August 2018

Peter,

I was just changing cosine to sine in your file. But at that time the solution is not converging. An error is showing in mesh generation even changing anything in your file (after cleaning generated data).

If I drag structural solution as per your suggestion (in part 4), will it make a significant difference in the result?

peteroznewman posted this 17 August 2018

Hello Masud,

1) Are you using a global mesh size setting in the Mesh details or a mesh Sizing control? If the element size is small enough, either method will succeed, but you might have a lot more elements than you want to wait for the solver to process.

2) Make a screen snapshot of the equation. If you have numbers for A, pi, and f and you type time instead of t, you should be all set.

3) Translational joints are always along the X axis, but you can edit the Coordinate System that is underneath the Joint definition and point the X axis in any direction you want.

4) In Workbench, if you drag a Static Structural Solution cell that includes Gravity onto the Setup cell of the Transient Structural, then you will have the Static Structural solution as the initial conditions for the Transient solution and Gravity will be present in the Transient solution.

5) I don't have any tutorial for vibrationdata, but I will take your questions here.

masud407 posted this 17 August 2018

Hello Peter,

Thanks for your response. Your file with cosine joint displacement is working. However, I am facing some problems while working on it:

1) I tried to refine the mesh size, but this message is coming every time "The mesh generation did not complete due to poor quality elements or incorrect input. Please try meshing with another mesh method or different mesh options."

2) As the equation is X=Asin(2*pi*f*t), I tried to insert sine function instead of cosine. But it wasn't working at that time.

3) In the definition of joint displacement, is there any chance to change the DOF from X direction to Y direction? I tried but could not found anything.

4) Previously, I fed gravitational loads with static structural before moving to transient structural. Now, f I start directly with transient structural, will there be any difference?

5) Can you provide me with any source/tutorial link where I can learn the post-processing in vibration data for the continuous frequency range?

peteroznewman posted this 17 August 2018

Muscle and Bone model is working by using a cosine displacement function.

Attached Files

• Liked by
masud407 posted this 16 August 2018

Thanks  Peter for your response. Previously, I used the same properties of muscle to simulate the simpler geometry. However, it is showing invalid now for this geometry.

Yes, you told me about the vibration data before. Once I am done with this simulation, I will start post-processing with vibration data

peteroznewman posted this 16 August 2018

Masud,

I have matlab and a free set of scripts with a nice GUI front end called vibrationdata. With that I could generate a sine signal with the amplitude and frequency I wanted, then I could double integrate that signal with another script.  The integration script can subtract the mean from the velocity before integrating the displacement. That would have made more sense from the point of view of a real shaker table experiment.

I will look at the material definitions for muscle and bone later today and make another post.

Regards,

Peter

masud407 posted this 16 August 2018

Thanks Peter. Yes, it was my mistake while calculating the force. I was trying to simulate your file with muscle (outer part of the geometry) and bone (inner part of the geometry) properties.  However, it is showing error and saying invalid muscle properties. Is there any way to do the simulation with muscle and bone properties by changing mesh size/step size? You can find the properties of muscle and bone in my previous file that I attached.

My target is to provide vibration at a certain frequency and find the acceleration/stress distribution at any point of the geometry. Then I need the graph for a continuous frequency range (for example from 20 Hz-50 Hz). How did you get the acceleration vs time/ velocity vs time diagram?

peteroznewman posted this 16 August 2018

Attached is an ANSYS 15.0 archive that has a Joint Displacement function of a 10 mm amplitude.

The system solves and here is the resultant velocity.

Some of the noise in the initial 1 second could be reduced by using a smaller time increment, or adding more damping to the model.

Regards,

Peter

Attached Files

peteroznewman posted this 16 August 2018

Here is the deformation result from Transient Structural, 12.2 m of displacement.

I expect you wanted the displacement or velocity to have a sinusoidal profile, about a zero baseline displacement.

Regards,

Peter

Attached Files

masud407 posted this 16 August 2018

I have uploaded the file once again. I am using Ansys 15. Please let me know if you can't open/find the file.

peteroznewman posted this 16 August 2018

Looking at your Transient Structural, you have nothing to guide the body that the force is applied to. Therefore, the force will cause the mass to accelerate but also to rotate about its Center of Gravity.  Since you were earlier talking about a shaker table, I will add a Joint so that the body can Translate along the Y axis.

The mass of the 3 bodies combined is 0.082 kg. You are putting a sinusoidal force of 739 N. Using F = ma reveals the peak acceleration is 921 G.  That is an obscenely high acceleration.  I edited the force to 0.803 N so the peak acceleration was 1 G. With a 1 G acceleration at a 0.5 Hz freqency, a hand calculation of the velocity and displacement is plotted below. The peak velocity is 6.24 m/s and the total displacement is 12.5 meters!  Instead of applying a force to a mass, you can just apply the displacement you want to the joint.

Regards

Peter

• Liked by
masud407 posted this 15 August 2018

Hello,

I have attached my wbpz file. I am trying to apply a sinusoidal load to the structure. Although I need to insert the properties of muscle and bone, I have allocated steel properties for the generalized purpose. An error is showing which says "The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information." Can anyone of you please give me some suggestion to solve the problem? thanks in advance.

Attached Files

peteroznewman posted this 17 June 2018

Take a look at the ekill script in this discussion.

A different model is attached below.

Attached Files

masud407 posted this 17 June 2018

For my problem, where to put the command? Can you please provide me any materials for learning the basic command relevant to my problem? Thanks

Attached Files