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

# Need To apply external vibration

- 1.6K Views
- Last Post 02 July 2019
- Topic Is Solved

What does you question have to do with ANSYS simulation software?

To shake an object, you can use a permanent magnet shaker, a power supply and a controller or signal generator.

If you are at a University in the USA, you need to have approval from an Institutional Review Board (IRB) before any human testing begins.

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?

It's the same thing on a bigger scale. There are shaker tables that you can stand on or bolt a seat to and shake on a vertical axis.

The type of shaker table actuator depends on the frequency you want to apply. If you want to go down into the single digit number of Hz, between 1 and 10 Hz, then you must use a hydraulic actuator. Lansmont is one company that makes hydraulic shaker tables. If your lower limit is above 10 Hz, then you can also use electro-dynamic shakers such as ones from Sentek.

Here is an image of a seat bolted to the armature of a shaker with a manequin strapped to the seat. The armature is driven by electromagnetic coils that are in the drum and powered by the power supply in the cabinet.

Thanks for your reply. I want to simulate the whole process in ANSYS. How can I apply the shaker vibration in ANSYS? Can I do it by using ANSYS static structure module?

You could use a Transient Structural system to simulate a shaker table. You could also use Harmonic Response since you are applying a sinusoidal input.

I tried with Harmonic Response where I could apply force/acceleration as constant/tabular format. However, I could not apply acceleration/loads as function of time. How can I do that in Harmonic response module? What is the difference in applying load in static structural module and harmonic response module?

thanks.

In Harmonic Response, when you apply a Load such as a force or acceleration, you are specifying the amplitude of the vibration. It is assumed that the load is sinusoidal with time. During the solution, the frequency of the sinusoidal vibration is stepped from the minimum to the maximum frequency specified in the Analysis Settings. In Static Structural, the load is a fixed static value.

Thanks for your reply. For example, If I want to apply a sinusoidal load in a particular direction having frequency 30 Hz, amplitude of .4 mm, then what should be the magnitude of force in the harmonic response module? For static structural module, what if I use this formula F=ma for having the solution? Does that mean that I will get the solution for a particular frequency only?

Apply a displacement of 0.4 mm in the desired direction. In the Analysis Settings, you can specify 30 Hz for this Harmonic Response.

The maximum acceleration of a point vibrating at 30 Hz with an amplitude of 0.4 mm is 14.2 m/s^2 or 1.45 G. You could use this acceleration to determine the force required to move a mass m at that vibration frequency, but that is a harmonic force. A static force would have a different result on a structure.

How can I specify 30 Hz in the analysis setting? Does it mean that I need to keep the minimum range 0 Hz and maximum range 30 Hz in analysis setting? Moreover, in the harmonic response, If I apply 14.2 m/s^2 acceleration, then do I need to apply the equivalent force or displacement separately?

,

Typically, in a harmonic response, you want results at many frequencies, but if you are only interested at one frequency, you can set the minimum and maximum range to 30 Hz and request 1 result.

If you know a point on the structure vibrates with a specific displacement amplitude, then you can apply that one displacement to that one point and the stiffness of the structure will deform the rest of the structure. Say you had a cantilever beam, and one end is fixed, and the other end is connected to an actuator that raises and lowers the tip by +/- 0.4 mm, then you would fix the one end and apply a tip displacement of 0.4 mm and the harmonic analysis will show you the displacement of the rest of the cantilever when the tip is vibrating at 30 Hz. If 30 Hz is near the first natural frequency of the cantilever, then the center of the cantilever will have a much larger displacement than 0.4 mm if the damping is low.

If you want the entire structure to experience an acceleration load like it is bolted to a shaker table, then just apply the acceleration. You might have a cantilever beam fixed at one end and simply supported at the other end. If 30 Hz is near the first natural frequency of the cantilever, the maximum displacement. will be near the center of the cantilever.

I really appreciate your help. I tried to put 30 Hz at both minimum and maximum range, but ANSYS is not taking the same HZ at maximum and minimum tab. I was following the steps (method 2: Direct Acceleration Method) form the following link:

https://caeai.com/sites/default/files/WB%20harmonic%20shaker%20table.pdf

I am confused about applying static loading in static structural module before going to modal and harmonic response analysis. Why do I need to preload the structure before modal and harmonic response analysis?

I come to know that harmonic response is for linear system. How can I tackle the nonlinear systems in the harmonic response analysis(for example: I need to apply 30 Hz to a nonlinear system)? I am sorry for asking such kind of novice questions as I am a new ANSYS user. Thanks

If you put 0 and 30 Hz and request 1 result, you will get just 30 Hz, but as I said, most users want to see how the response varies across a range of frequencies.

Feeding a Static Structural Solution into a Modal Setup allows the modes to be calculated after an initial stress is developed. The classic example is a guitar string. It needs a high tension before it will have a first natural frequency in the audible range. A large flat circuit board will stiffen slightly as gravity pulls a belly into the center of it. But if you have a structure that does not stiffen due to applied loads, you can skip this step.

You are correct that harmonic response is for linear systems only, so you can't have a frictional contact opening and closing in the model. If that is important, then you have to use a Transient Structural model, and not one linked from a Modal analysis system, but a stand alone one. Then you apply a sinusoidal acceleration-time history and simulate several seconds of time to let the transient portion of the response die away due to damping, while the periodic response settles in.

You can link a Transient Structural model setup cell to a Static Structural solution cell if you need to tension that guitar string before the transient portion begins.

Thanks for your reply. As my system in nonlinear, I used a Transient Structural cell liked from a Static Structural cell. *In the Transient Structural cell, I used sinusoidal load/acceleration* as a function of time for a particular frequency (For example: I calculated the equation with 30 Hz and put it in the function tab) and got the output. Now, If I want to see how response varies across frequency, then can I use modal and Harmonic response analysis for that? If yes, then what will be the applied load/acceleration value that I need to put in the Harmonic Response module?

You will create a copy of that system and replace the equation for 30 Hz with an equation for 60 Hz or what ever frequency you want and run that transient solution.

Okay, I understand that manual process. But if *I want to draw a continuous plot of freq vs displacement (similar to Harmonic Response), Then will it be possible to draw for the nonlinear system except doing it manual process (inserting separate formula for different frequency)?*

If you create an input Parameter for the frequency value, and use that Parameter in your equation, then mark the maximum displacement result as an output Parameter, then you can go into the Parametric Set window and make a table of input Parameter values of all the frequencies you want in the plot and click Update Design Points and let the solver run once for each row in the table, filling out the output Parameter value in the table. That would automate the creation of the plot of max. displacement vs. forcing frequency.

Thanks for your reply. As I need to apply sinusoidal force at a particular frequency (F=ma=m*w^2*Asin(w*time), w=2*Pi*f), therefore, I applied force as a function of time. However, there is no option(rectangular box where P appears) for parameter setting for the force which is expressed in terms of function/tabular data. For the force with constant magnitude, parameter set option appears only. What should I do now?

I don't see a simple way to automate multiple Transient Structural solutions with input force-time histories that each have a different frequency. It may be possible with APDL programming.

A far more common need is addressed for linear systems in the Harmonic Response analysis where the entire system is built to automate obtaining results over a range of forcing frequencies. How large is the difference between a full Transient Structural solution and the Harmonic Response solution?

Actually, I want to apply vibration to the lower part of the human body. According to the lumped model, the lower body part acts like a nonlinear system. As parametric setting does not suit with the time varying force applied in static/transient module, as per your suggestion I need to use APDL programming. Does it mean that I need to work with ANSYS APDL instead of workbench or apdl commands in ANSYS workbench?

I use APDL scripts that run in Workbench as Command Objects, but I don't have the skill to write an APDL program. This seems like a simple loop to go through a range of frequencies. Other members might be able to give some guidance on that.

You are more likely to get some help if you provide a specific model that you want to automate. An open ended question with no specific example poses a significant barrier to someone who might be able to help.

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

Take a look at the ekill script in this discussion.

A different model is attached below.

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.

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

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

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 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

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?

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

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

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

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?

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.

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?

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.

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.

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

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.

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

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?

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

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

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

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.

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

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?

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

Moved your new question to a new discussion.

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

Hi jinyan,

Please open a **New Discussion** to discuss your vibration analysis.

Regards,

Peter

##### Search

##### Change Language

##### Categories

##### This Weeks High Earners

- rwoolhou 103
- abenhadj 86
- peteroznewman 79
- violet998 20
- jj77 19
- SandeepMedikonda 17
- BenjaminStarling 11
- Soldojohn 11
- HuiLiu 11
- brmaciel 9