My name is Antoli and I'm an engineering student from Spain. I'm involved in a project about ultrasounds in my university and I'm trying to simulate the ultrasonic equipment. This equipment is composed of a piezoelectric transducer (energy source), a booster and a sonotrode. The transducer has fixed frequency and fixed amplitude, and the booster and the sonotrode only amplify this amplitude. Both have to be tuned in the transducer frequency.
I know that simulate the piezoelectric transducer is very difficult, for this reason my idea would be to replace the transducer by its corresponding movement (amplitude: 20um, frequency: 20kHz) in order to get the amplitude at the end of the sonotrode.
I've done a simple natural frequency analysis but this isn't a correct approach for my application.
Could you give me some advice to simulate my equipment? Which would be the best way to success?
Thank you very much!
Solved! Go to Solution.
You can indeed do this by natural frequency (modal) analysis. If you know (or can determine) the gain of your booster Gb, then the input amplitude to the sonotrode Uinput is 20um*Gb. For the following example, assume Gb = 1.5 so Uinput = 30um.
With the above information you can run a modal analysis of the sonotrode alone. (Depending on your circumstance you may want to include the booster. However, this is usually not needed unless you are concerned with the booster's isolation mount or unless you don't know the booster's gain.)
After you run the modal analysis, when you display the desired modeshape you will see the relative amplitudes. Rotate the model until you can see the center point where the booster would attach (generally the center of the sonotrode's input face). Right click on this node and then choose Inquire\Results. Record the displacement value in the direction of the booster's axis (i.e., in the direction of the input amplitude to the sonotrode). For example, if the booster's axis would be in the Z direction, then record DZ. This displacement is the reference displacement to which all others will be compared. For the following example, assume that this value is 13.6 (your value will be different).
Now you can compute the relative amplitudes at any other location on the sonotrode. For example, at the center of the sonotrode's output surface (the face) you may click and find a DZ value of 67.2. Then this location has a relative amplitude of 67.2/13.6 = 4.94. The actual amplitude will be 20um*1.5*4.94 = 148um (i.e., 20um transducer output * booster gain * sonotrode relative amplitude). If the sonotrode is symmetric then the transverse displacements at the center of the sonotrode's face will be small.
You can use this same method for any other location on the sonotrode. For example, at a corner you might have:
DZ = 58.3 ==> relative amplitude = 58.3/13.6 = 4.29 ==> 129 microns
DX = 4.7 ==> relative amplitude = 4.7/13.6 = .346 ==> 10.4 microns
DY = 5.2 ==> relative amplitude = 5.2/13.6 = .346 ==> 11.5 microns
You may want to make the following interface settings:
1. Set the "Results options" to "Absolute value". This will then typically display a dark color at the node(s) so that the node(s) can easily be located.
If you need the stresses then you will have to also run a frequency response analysis after the modal analysis.
Thank you very much for your answer, it helps me a lot. However, I obtained a logical results without setting the "Results options" to "Absolute value", basically because I'm not able to find where can I set it.
In the new ribbon interface click "Results Contours", then "Settings" dropdown list, then "Absolute value".
In the "classic/old" interface click on "Results options', then "Absolute value".
To change the interface:
- From the ribbon interface click "Tools", then "Application options", then in the "General Information" tab "Ribbon style" will be checked. Click on this anyway and it will ask if you want to change to the Classic interface. Click Yes and "Cool look" will then be checked.
- From the Classic interface click "Tools", then "Options", then in the "General Information" tab click "Ribbon style".
Personally I like the Classic interface because it often needs fewer clicks.
I would be very grateful if you could help me with another small problem. I would like to force a sonotrode and a booster to vibrate at 20 kHz and then evaluate the amplitude. I think that with the natural frequency analysis type I can't do it. Which is the correct way to success?
Have you been able to extract the natural frequencies of the booster-sonotrode stack?
Do you want to know the amplitudes or do you also need the stresses?
Must the system vibrate at exactly 20000 Hz or will you be operating at one of the natural frequencies. (Unless you adjust your model very carefully, the primary natural frequency will probably not be at exactly 20000 Hz. For example, although your nominal frequency may be 20 kHz, you might find that your model tunes to 19912 Hz, which could be quite acceptable. Also, the performance of your manufactured stack will likely differ somewhat from the FEA results (e.g., slightly different material properties, effect of temperature during operation, effect of joints, etc.) In addition, the sharpness of the resonance for a typical stack means that operating only slightly away from the natural frequency will cause greatly reduced amplitude. This is why the power supplies (generators) are usually designed to track the frequency. Therefore, for FEA it is better to assume operation at the extracted primary natural frequency (assuming that it is reasonably close to the nominal) rather than at exactly 20000 Hz.)
If you can operate at the primary natural frequency then you can apply the same method as previously discussed. In this case, however, all amplitudes would be scaled relative to the amplitude input to the booster rather than the input amplitude to the sonotrode.
If you need to operate at exactly 20000 Hz, regardless of the primary natural frequency, then you must use Frequency Response Analysis. (I can explain this further if you need.)
Absolutely. I was able to obtain the natural frequencies; your help was very useful. However, I observed that when you change the length of the sonotrode and run the natural frequencies mode, then you can't extract the performance of it at 20 kHz. So now, I would like to analyse what happen with the nodal planes and the amplitude if we fix the frequency (20 kHz).
For the moment I'm not interested in the stresses because the geometry of the booster and the sonotrode are very simply, and I think that I won't have any problem related to fractures when I manufacture and test them.
My ultrasonic generator works in a narrow range of 19,4 - 20,4 kHz, so if I don't do a correct simulation then the sonotrode and the booster will not vibrate. It could be really interesting for me if you were able to explain me the Frequency Response Analysis.
It's really interesting what you are explaining me.
Can you upload your current model without the results. (In the classic interface: File\Archive\Create --> creates an archive .ach file.)
What version of FEMPRO are you using?
You will find attached my model (booster + sonotrode).
I'm using the 2012 version.