# Lamb wave simulation - Problem with high Frequencies

Hi

I have prepared a very simple model in abaqus which is an Aluminum beam under A0 lamb wave. It wors perfectly with low frequencies andthe amplitude plot shows a clear one in various control points.

But when I increase the frequency to 200khz that nice and neat plot is not obtained. I have attached two plots 1-excitation wave 2- amplitude on control point

could you please advise as to why this happens on high frequencies and what is the solution to this ?

### Re: Problem with high frequencies

The obvious first question would be: Is your mesh fine enough to be able to handle these frequencies? The mesh you used for low frequencies might not be good enough at 200K Hz.

What are the bulk viscocity parameter you have set? Are you keeping it at the default 1.2 value or did you make them zero?

### Hi Bhisham Thank you for

Hi Bhisham

Thank you for your reply. I have tried various mesh size from 1mm ( 0.001) to 0.2mm ( 0.00002m) but got the same results. regarding bulk viscousity I am using the default value put by Abaqus and have not changed them.

Cheers

### You may see the following

Hi,

You may look into the following things.

1. Excitation of Ao mode - You have to give a required profile across the thickness of a plate to excite a required Lamb mode. If you do not give this profile, other modes will also get excited.

2. Is the excitation based on displacement or force?

3. Check - does the selected frequency falls in dispersive region?

4. Check any other modes exist at that frequency

5. Follow Blake's and CFL criteria for spatial discretisation and temporal discretisations, respectively.

6. Take responses (in-plane and out-of-plane) at other locations also. Compute group velocity of tail wave group. Check the group velocity matches with any othe modes excisting at that frequency.

Regards,

### Hi Ramadas Thank you for

1- In order to generate lamb wave I am applying the displacement on the surface of the beam which is 6mmby12mm. How do I give that profile ?

2-As I mentioned the excitation is based on displacement.

3-How would I check whether the frequnecy falls into dispersive mode or not ?

4-According to other software and sinceI am using Aluminum 200khz s lower than cut off frequency and therefore I don't think any other modes exist.

5-I ll study more about that. thanks.

6-could you explane more regarding ths ?

Regards

### Re: Problem with high frequencies

Hi,

The best way to choose the mesh size is to choose it according to the shortest wavelength in  your simulation. About 10 elements per wavelength should be good enough. I haven't done any calculations, but your mesh dimension seems to be fine enough (at a glance).

Ramadas makes some very good points. You are sending a modulated pulse, so it's quite narrow banded in the frequency domain and I don't think dispersion is affecting your results. I notice that you are comparing the signals at different times too. Why is that? One way to check for dispersion would be to look at the pulse at two different points along the beam. If there is dispersion, the wave profile wouldn't be the same. That's essentially what Ramadas is suggesting too in point 6.

The region ahead of your actual pulse shows some disturbance too. That is certainly spurious since none of the waves would be propagating that fast. What is the time step chosen? Make sure that you tell Abaqus to choose the time increment element by element. If you have access to Cook and Malkaus's FEA book, turn to chapter 11 where they talk about the Courant number and also give an example problem. That should make things a bit clearer. I am assuming you are using Explicit. Also, make sure that Abaqus is solving using double precision. Also try increasing the magnitude of your input pulse by an order of magnitude.

It's always a good idea to add a bit of numerical damping in your system when solving at higher frequencies. Add some global damping; just enough to not affect your pulse too much.

- Bhisham

### Some more responses required

Hi,

Thanks Bhisham.

Hi r_1159,

You mentioned that displacement was given over 6 mm X 12 mm. Could you please elaborate this?

What's the thickness of beam?

To check whether the frequency falls under dispersive or non-dispersive region, you have to plot dispersion curves

(phase velocity vs frequency at a given plate/beam thickness or phave velocity vs frequency-thickness product)

(a) If you are giving in-plane excitation on the surface, (x-direction, which is the direction of propagation) then, So mode with high amplitude will generate.

Moreover, Ao mode will also generate.

(b) If you are giving out-of-plane (z-direction - beam thickness direction) Ao mode with high amplitude will generate. And also, So mode generates.

If (a) is true, then high amplitude wave group is So and wave group at tail is Ao. Note that So travels faster than Ao mode.

Displacement time hisorty shown in the second figure is in-plane or out-of-plane? Could you please some more responses taken at other locations

away from excitation point?

Thanks and regards,

### Thanks you Bhisham for your

I am simulating an Aluminum beam which is 1.04m X 12mmX0.2mm.To excite A0 lamb wave I created a cut at 6mm from one end of the beam and appied the wave on the top surface. As I mentioned the wave is excited by applying out of plane displacement so the excitation surface is 6mm(cut)X12mm(width. To calculate the group velocity I created various control points and I got pretty good results for low frequencies (lower than 200khz). The ones you see on plots are located at 0 and 25cm. So the first point is located at excited surface and the second one is at 25cm from the forst one. I am using low amplitude to get clear signals I havealso used higher amplitude which does not give me good resutls.

The plots are out of place displacement.

So in this case I am folowing (b).

I have checked other points as well and as the control points get away from the excitation surface more mixed pulse are obsereved and the amplitude plots gets messy.This problem is not obsereved in low frewuencies and I am getting very clear and nice plot for A0 lamb waves with low frequencies.

I think there might be some issues with the way I am applying Ao mode. In your previous comment you mentioned that I need to give a profile through the thinckness of the beam. How would I do that? do you mean I have to create several cuts throughout the thicknes of the beam and apply the diosplacement to each layer?

To Bhisham: I am using Explicit analysis and the wave time steps are 1e-8 Secs. When defining step in Abaqus I am not changing any parameters in time step. The mesh size is very small and is smaller than 1/12 of wave length. How can I tell Abawus to use element by element time increment ? This could be a solution to my problem as well.

Are there any parsmeter or any tricks in Abaqus that could possibily improve the results ?

Thanks

### Re: Lamb waves

Hi all,

Haven't worked in this area, and probably should keep quiet, but it anyway is an interesting discussion, and so...

I think, dispersion is not the main issue here.

There are two main features to the second plot:

(i) A certain low frequency component arrives at the control point before the main pulse does. It does so with a very small amplitude initially. But it grows slowly, and then persists with a more or less the same amplitude for long time after the main pulse has passed by the control point.

(ii) There is a small "appendix" of a group of waves, somewhat similar to those in the main wavepacket but about 10--20% of the max amplitude, which arrives immediately after the main pulse does. The later half of the appendix is similar to the main pulse, but the earlier half shows something like changes of phases, probably a result of the superposition of the main pulse with the "appendix."

The first feature may have either to do with a physical effect (say dispersion, resonance, whatever) that is inherent to the range of the material properties and the frequency selected, or it may be due to numerical dispersion. Numerical dispersion, I think, is unlikely here. Or, let's say, I would be suprised if that turns out to be the main cause in such a simple case modeled with so established a piece of software. So, IMHO, it is more likely that this is not a numerical artifact; the model is showing something physical here. (Can't avoid my bias for the real usefulness of Computational Science and Engineering!)

As to the second feature, it makes one think of things like reflection, doesn't it? Is there any (weak) reflection that slips in by any chance? And, if not that, then as Ramdas pointed out, it has to be the other mode. (On second thoughts, I think this is going to be the case---a reflection wouldn't decay so fast.)

So, r_1159, I think that sharing a drawing showing all the relevant deails would help a lot here. In the drawing, please include not only the reference frame and the geometry and dimensions of the beam, but also show/mark out the following in it: (i) the location and the nature of the support(s), (ii) the region where the excitation pulse is applied, (iv) the direction(s) of propagation (BTW, do you model with a simple plain wave or with a complicated profile?), (iii) the location of the control point(s).

As I said, I don't know this area, really speaking! Just jumping in out of a general interest. (Hey, this is just a blogging forum, OK?) ... Will be interesting to learn what turns out to be the real cause, here. So, over to you all.

--Ajit

- - - - -
[E&OE]

### What is this six mm cut???

Hellow Dr Ajith Sir.

Hi r_1159,

I haven't understood clearly about this six mm cut. Is excitation point away from one of the ends of beam? If so, as Dr Ajith pointed out, it can be a reflection from the end.

One more thing is, check is there any time separation between the wave groups with distance of propagation.

Apply out-of-plane displacement right on the face (12 mm width X 0.2 mm thick) of beam.

Each Lamb mode has two displacement components (across beam thickness), u and v, and they are functions of x and z.

u = u(x, z) and v = v(x, z)

Spatial distribution of u and v can be obtained from dispersion relation. If this is available, one can apply across the thickness to excite a particular Lamb mode.

If you have any problem in simulating, please send me the details of your model and material properties. I will do it in ANSYS.

Best wishes,

### Hi to Ramdas

Hello, Dr. Ramdas,

Nice to be back in touch again!

Looking at the latest comments below, it's the other mode, not the reflection.

Cheers!

--Ajit

- - - - -
[E&OE]

### Excitation

And thankvyou Ramadas for replying my post. I just explain the 6mm cut more. The excitation surface is 6mm long and is located from 0,0.0002,0 to 0.6,0.0002,0 meaning that i am applying out of plane displacement to top surface of the beam from one end and the control point is located 25cm from that end so the extra pulse cannot be the reflected wave from the other end of the beam as there should be a time delay between main pulse and the reflection pulse. But what i understood from your comment is in order to generate A0 lamb wave you apply out of plane displacement to the cross section of the beam while i am applying the displacement on top surface of the beam. Is this what you mean?

I have done the simulation in Abaqus so please let me know if i can send the input file to you for your review.

I am applying the displacement on the top of the beam to simulate piezoelectrics.

Thanks

### Re: Problem with high frequencies

I must say that I misunderstood your problem a bit. The way you are exciting the wave is throwing me off a bit. I am still not sure what the 6mm cut is all about. I think Ramadas made the same assumption as me, that is you are exciting the beam at one end. If you were doing that, there would be not possibilities of reflections coming in. But that seems to not be the case.

1. Your mesh size is more than adequate. In fact, back of envelop calculations tells me that your mesh size should be able to handle frequency upto about 75000 khz without any problem. You may reduce your computational time by increasing your mesh size. Unless you are in a rush, I would change the mesh size to about 0.005 m or 0.0025 m and get the entire displacement field as the output. You can then use your simulation to understand what is going on in your problem.

2. Time step: Again, a rough calculations gave me a critical time step of about 4e-9 for your mesh size (Element length/ max wave speed). I am using wave speed of 5000 m/s, which I think is the longitudinal wave speed in Al. Typically, a time step only slightly less than this critical time step gives the best answer. A courant number (Find out more about courant number) of about 0.96-0.98 is usually a good choice. Considering your time step, this might be affecting the accuracy of your results.

3. Distortion in the main wave tail: There are two parts to this: 1. The wave shape towards the end of the pulse and 2. The remnant disturbance after the pulse has passed through.
The disturbance after the wave has passed through should most likely be affected by the damping factor after you changed it. Was that the case? I suspect this part to simply be numerical noise. What is more interesting, and your main issue is the first part.

Admittedly, I don't understand the 6mm cut buisness very well. Since it is not at the end, it has to be either reflections or a second mode is being generated. Lamb waves are a complicated thing to analyze. If you can't solve for the entire field, take output at a few more locations, one nearer to the excitation and one further away and see what happens. Do post the results here too if you can. It's an interesting phenomenon. Like Dr Ajith, I suspect that this will turn out to be an additional mode generated due to your loading.

You can email me your input file if you want. I might not get the time to look at it immidiately though.

Bhisham

Hi Bhisham,

A correction. It was Ramdas who first pointed out the other Lamb mode here, not me.

--Ajit

- - - - -
[E&OE]

### Hi Bhisham Lots of

Hi Bhisham

Lots of interesting points! Thanks a heap.

I am gonna post more plots tomorrow and will send the input file to you as well. My email address is r_ 1159@lycos.com so I would be thankful if you could send an email to me so that i reply ythat with the input file.

Sorry as i misunderstood you and Ramadas with 6mm cut. I will post a screen shut from that tomorow and will upload here to explain how im generating wave. But to clarify,  the wave is excited in one end of the beam by applying out of plabe displacement on top surface of the beam withthe lenght of 6mm and width of 12mm and i have defined this as a boundary condition. The beam lenght is 1m and its width is 12mm and

thickness is 0.2mm. The 6mm cut is a cross section cut to create the required geometry for applying the wave on top surface of the beam and is

not a structural cut. So you can ignore this cut as it is a geometry cut only.The control point is 25cm from this end. I have tried many mesh sizes and yes you are 100% correct as 5mm mesh size is more than enough. I have also tried many models with different lenght and thickness and am getting the same results in high frequencies.I feel there might be some issues with my time increments. I used element by element time increment

Could you tell me how i can change the value of time increment in Abaqus ? I can't find that in Step. Then i will change the time increment and will post the results here as well.

Thanks

### Apply on the face of beam

Hi,

Good points from Bhisham.

Hi r_1159,

I agree with Bhisham. This six mm cut is complicating the things.

What you understood is correct. Apply out-of-plane displacement on the face (0.2 mm X 12 mm) of beam.

This approximation on displacement pattern to excite Ao mode is true, if the thickness of beam is less. This simulation will give you a basic idea about propagation of Ao mode.

Moreover, take responses at some more locations. Response at location doesn't help you much.

If you take some more responses, then, you get an idea about increase (or no change) in time separation between the two wave groups.

Recently I was simulating propagation of Ao mode in a 2 mm thick alumiminium plate (plane strain condition).

Mesh size was 0.5 mm (square mesh, eight node element) and time step size was 50 nano sec (Ao mode velocity is 2500 m/s approx).

I gave displacement profile to excite Ao mode. I could get nice results.

Best regards,

### Hi Ramadas & Bhisham Just a quick

Just a quick question, do you use shell or solid for your simulation ?

### SOLID

Hi,

I used SOLID (2D or 3D depending on probelm) elements.

Best regards,

### Re: Problem with high frequencies

Thanks for sending the CAE file to me. I used quadratic elements and switched the non linear geometry off, but it doesn't affect the results. Your output is correct. To understand what's going on, I had to take the output at a further location, node 5663. Here, you can clearly see the two modes seperating out since they travel at different speeds. So the answer to your problem is: You have two modes at that frequency and that's why your results look different at higher frequency.

### Problem posting the image

I was trying to post the image file showing the separation of the two modes, but I am having problems doing it. Admittedly, I haven't uploaded an image before so it might be just me.
I tried the image option in the formatting window, but I get a "Callback browsed error". And simply copy pasting isn't working either.

I have emailed you the image, if you can upload it here for the rest to see, then it will be helpful.

### Plot by Bhisham

Thanks a lot Bhisham. Well done! Here you can find the plot. Thanks for taking the time for reviewing my model in depth and I appreciate your sense of sharing information with others. I just realised the problem day before yesterday. What I am understanding is I am using a beam which is indefinite in lenght but DEFINITE IN WIDTH and this causes a new mode or it can be reflection from beam boundary at that frequency and my second mistake was that I was comparing my results with dispersion curve that was obtained for a plate which is indefinite in length and width and this was what made me bussy for a week.

I have a question and I would appreciate if you could answer. While your work was great to take a plot in other location I realised that you have used a very small amplitude which is 1e-21. could you please explain the reason as to why you used this much small amplitude factor ? Also could you please confirm if my understainding of boundary causing the issue is correct ?

Once again I thak you for contribution to this post

Cheers

### Re: Problem with high frequencies

The amplitude reflects the value which was input by you. I did not change the input in any way. I don't think the boundary is causing the issue. It's just another mode inherent in the beam.

Refer the books on wave propagation in elastic solids by Achenbach or by Graff, or the book on wave propagation by J.F. Doyle.  Prof Doyle discusses this behavior in his book.

### Hi Bhisham Thank you for

Hi Bhisham

Thank you for your reply and yes I had defined the scale factor but had forgot as worked on so many models. I made a new model which is a plate with the same thickness and 60x60xm size. applied the wave on the center of the plate and got very nice results on every nodes of the plate. No disturbing pulse at all that is why I am guessing that could be generateed by beam boundary. The only difference between two model is their bouundary consition. However since you have more knowledge and experience than me I am very interested to understand the reason according to your references.

Cheers

### Reason for more than one Lamb mode?

The reason for the appearance of more than one Lamb mode?

There will be molecular/atomic/quantum level explanation, I am sure. In the continuum theory, we homogenize everything and also further idealize (or "go up in the scale" also for) the boundary conditions, and so, I am not sure if you would get any explanation other than the principle that if the initial and boundary conditions are general enough to allow for appearance of more than one mode, then they all will.

The situation seems somewhat analogous to the equipartition theorem of statistical mechanics which basically says that if the laws of thermodynamics allow a system to exist in 'n' number independent energy-carrying modes, then it will do so as a superposition of all those modes with equal energies in each. ... BTW, don't take this formulation verbatim; it might be too vague; I just wrote it on the fly without referring to any book or so.

... And don't give the theorem too much respect either. It's not as helpful as it sounds; it sometimes merely shifts the place of the pain. The pain now is in knowing what might qualify as a valid and independent energy-carrying "mode," and further, in not missing out on any possible mode while enumerating the modes. ... There are times when the theorem doesn't really help any more than what Murphy's II law would: if many things can go wrong at the time of a single demonstration, they all will!

Anyway, I am glad to see the basic issue of this thread get resolved. Thanks, Bhisham, for your inputs.

And, in general, I would like to know if there is any classical continuum/solid mechanics principle (applicable to a single body) that is analgous to the equipartition theorem of statistical mechanics (applicable to many particles/bodies).

Best,

--Ajit

- - - - -
[E&OE]