Finite-element analysis of a 6" woofer

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
A 6" woofer will be analyzed by finite-element software. FE results will be compared to test data of a physical data.

It is a typical woofer obtained from a factory mainland china. The main purpose of this study is to see how close the virtual driver to the physical driver.

3D drawing of the driver is not available from the factor. On the other hand 2D drawing in pdf and kit of parts are given. 3D drawing is then created based on the 2D drawing and components.

The 3D geometry is shown in the graph below. Roll-surround characteristic will be investigated first.

Initially, linear rubber in the material library is used for simulations.

At first, stiffness vs displacement, kms(x), of the surround is of interested. Although linear rubber material (linear elastic) is assumed, geometric nonlinearity will result in nonlinear kms(x). Therefore, nonlinear static analysis is employed.
 

Attachments

  • 6inch woofer1.png
    6inch woofer1.png
    67.9 KB · Views: 552
Last edited:
Outer flange of the surround is glued to the chassis. Hence, its boundary condition in the software is fixed. At this stage of analysis, cone (diaphragm) is assumed a rigid body. The inner surround flange can only displace in the vertical z-axis direction. An evenly distributed force (BC) is added to the inner flange as shown in the axisymmetric model below. This model is used for nonlinear static analysis.
 

Attachments

  • 6inch woofer 4.png
    6inch woofer 4.png
    53.2 KB · Views: 541
Nonlinear static analysis result is presented here. Rubber mechanical properties: elastic modulus 6.1 MPa, Poisson's ratio 0.49, mass density 1000 kg/m^3.

The graph below is showing the surround model moving into the motor. The maximum displacement is 11.35 mm. The curve shown below represents load scale (force) vs displacement. This is equivalent to typical kms(x) graph where force = stiffness x displacement. We can see the curve is pretty much a straight line up to ~8 mm.
 

Attachments

  • 6inch woofer 5.png
    6inch woofer 5.png
    17.4 KB · Views: 531
  • 6inch woofer 6.png
    6inch woofer 6.png
    51.2 KB · Views: 522
Last edited:
FEA data: displacement vs force load can be curve fitted (n-th order polynomial) in numerical tools such as octave, scilab and matlab. Target Kms(x) is the first-order derivative of the polynomial as depicted below. Stiffness is nearly a constant in the region of -5 mm to 5 mm.
 

Attachments

  • 6inch woofer 8.png
    6inch woofer 8.png
    7.1 KB · Views: 513
A 6" woofer will be analyzed by finite-element software. FE results will be compared to test data of a physical data.
It will be very interesting to see how you get on. You mention including acoustic radiation but do you also intend to include thermal effects?

A few years ago Scan-Speak got a number of companies to simulate a small wideband driver (I think) in order to evaluate modelling capabilities. I have had a brief google but failed to find anything. Is anyone aware of a link to any reports? The results were reportedly not wholly positive with the difficulties of incorporating sufficiently accurate damping being the main culprit (I think). Sorry about the vagueness but I am trying to recall the contents of an email exchange from a few years ago which I no longer possess and where this was peripheral to the main topic.
 
The Kms(x) shown in https://www.diyaudio.com/forums/multi-way/328373-finite-element-analysis-6-woofer.html#post5566049 is based on the rubber in the material library. It may not be a good representative of the actual rubber surround. We could measure hardness of the rubber and make conversion to elastic modulus.

An axisymmetric model with the cone is used for modal analysis for estimating the piston frequency. Using rubber in the library and given cone mass, piston frequency is 45.3 Hz as shown in the graph.

We need actual rubber elastic modulus to get good result. In contrast to static analysis, we need to obtain elastic modulus of the rubber under cyclic loading. Elastic modulus of rubber is not a constant but frequency dependent.
 

Attachments

  • 6inch woofer 9.png
    6inch woofer 9.png
    26.4 KB · Views: 112
Last edited:
We need actual rubber elastic modulus to get good result. In contrast to static analysis, we need to obtain elastic modulus of the rubber under cyclic loading. Elastic modulus of rubber is not a constant but frequency dependent.

This is where things get fun. Damping is important for drivers and speakers but, unlike mass and stiffness, it is difficult to model reasonably accurately. Not only is there damping within materials themselves but there can be significant additional damping/friction in joints.

There are a range of damping models for materials but the more realistic ones are often not implemented in general FEA codes. The adopted model will determine the number and kind of coefficients needed to represent the stress/strain/rate of strain/... relationship. It will also determine how much larger and slower the simulation will become. Which dynamic models does your FEA code support?
 
This is where things get fun. Damping is important for drivers and speakers but, unlike mass and stiffness, it is difficult to model reasonably accurately. Not only is there damping within materials themselves but there can be significant additional damping/friction in joints.

There are a range of damping models for materials but the more realistic ones are often not implemented in general FEA codes. The adopted model will determine the number and kind of coefficients needed to represent the stress/strain/rate of strain/... relationship. It will also determine how much larger and slower the simulation will become. Which dynamic models does your FEA code support?

Thanks for your comment.

To my knowledge, damping seems to be geometry dependent too. I measured stiffness and damping by means of bending (fixed-free cantilever) test of rectangular beam of the surround rubber. Damping obtained from the bending test and damping of the complete cone-surround are not the same.

The FEA tool supports typical proportional damping model and structural damping. It supports creep as well. Are these answers of your question?
 
Hi guys,

Let me update the driver type being studied. I don't have parts for the one with rubber surround, but for another 6" woofer with foam surround. Luckily, they are essentially identical except the surround material. I don't need to make changes to the already created models and just need to update the material properties.

Please see photos of the driver and its soft parts.
 

Attachments

  • parts 3.jpg
    parts 3.jpg
    118.8 KB · Views: 231
  • parts 2.jpg
    parts 2.jpg
    81.6 KB · Views: 237
  • parts 1.jpg
    parts 1.jpg
    113.7 KB · Views: 235
A rectangular beam was cut from the outer flange of the surround part. The beam was fixed a one end and free at the other end for bending test. Laser sensor measured the displacement of the free end. Vibration level was kept small in order to use Euler-Bernoullis (simple) bending theory to correlate elastic modulus to measured resonance frequency. The beam resonance frequency obtained is 55.7 Hz.

Vibration analysis package written by Tom Irvine was used to get elastic modulus. The GUI of the script is shown in the graph. Elastic modulus obtained is 5.5 MPa where mass density is 350 kg/m^3.
 

Attachments

  • Beam Bending 3.5x20mm 0.5V.png
    Beam Bending 3.5x20mm 0.5V.png
    78.2 KB · Views: 223
Paper cone mass density estimated is 910 kg/m^3. A quarter solid model was created to perform modal simulation. Together with the mass of dust cap and voice coil former, the mode 1 (piston mode) frequency is 33.4 Hz as shown in the graph.

We can verify this result later with the actual driver (spider removed).

The complete driver TS parameters are

FS 40.8715 Hz
VAS 11.3314 L
RE 3.9000 Ohms
QMS 9.7463, QES 0.8307, QTS 0.7655
BL 6.3000 T×m
dBSPL 81.7136
SD 1.327E-2 m2
CMS 0.4606 mm/N, MMS 32.9206 g, RMS 0.8674

L1kHz 1.3019 mH
 

Attachments

  • 6inch woofer 10.png
    6inch woofer 10.png
    95.1 KB · Views: 192
Using shell (plate) elements for complete cone-dust cap-surround modal analysis. Simulation can run much faster even with higher mesh density (not the one shown).
Plate and shell elements are different. There are also different kinds of these types of element which work well for some situations but not for others. The degrees of freedom they discard can be required near boundaries or where more general elements are used.

If you are not experienced using these elements it may be wise after you have built a full model to run a few checks to prove that you have not suppressed important degrees of freedom and have used sufficient resolution. That is, setup a representative simulation and repeat it using several levels of grid refinement everywhere, low and high order elements, elements that suppress no degrees of freedom and those that suppress ones considered unimportant,... and compare the results looking for differences.
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.