How to simulate speaker / crossover using OrCad

You can simulate the behaviour of a speaker and its crossover by professional speaker design software. In case you do not have access to these software, an alternative would be to use the SPICE simulation software to do the speaker simulation. Here I will demonstrate how to do this using OrCad. There is a demo version of OrCad release 10 which you can download from Orcad's web site to try.


Thiele-small eqivalent circuit

Before you can simulate your driver in Orcad, you need to calculate the eqivalent circuit for your driver unit. This circuit can be derived from the Thiele-small parameters.


For example, if a driver has the following Thiele-Small Parameters :

  Thiele-Small Parameters
Revc 5.8 ohms DC resistance of voice coil
Levc 0.55 mH voice coil inductance
Bl 6.5 T.m force factor
Qts 0.35 total Q
Qes 0.45 electrical Q
Qms 1.55 mechanical Q
Fs 37 Hz resonant frequency
Mmd 0.014 kg mass of cone + voice coil + etc
Rms 2.08 resistance of suspension
Cms 1.34 mm/N compliance of suspension
Sd 0.0136 sq.m effective cone area
Vas 0.0347 cu.m equivalent acoustic volume
Xmax 0.004 m linear travel of voice coil
FR 37 - 5000kHz frequency response
Vd 0.0005 cu.m driver unit volume displacement


Then this driver can be modelled with the following circuit :

Some of the circuit values above are already obvious. Veg represents the amplifier and is assumed to have no output resistance. The remaining values were calculated from,


Cmes = Mmd/(Bl*Bl) = electrical analog of driver mechanical cone mass
Lces = Cms*Bl*Bl = electrical analog of driver mechanical suspension compliance
Res = Bl*Bl/Rms = electrical analog of driver mechanical suspension resistance
Cmef = 8*po*Ad*Ad*Ad/(3*Bl*Bl) = electrical analog of air load on the driver unit's cone


po = air density = 1.18 kg/cu.m
Ad = effective radius of the driver unit's cone = Square Root of (Sd/3.14)


Some of these parameters can be look up from the driver's specification. This missing one could be calculated using the Unibox excel file. Unibox is a free tool that can help you to design speaker enclosure.

Speaker Driver Unit Simulation

After you created your driver models, you could start by testing if your driver model's impedance response is similar to your driver's actual impedance response. Now you need to familiar yourself with OrCad if you have not used it before. Here is a great Orcad tutorial that I suggest you to read if you have not used Orcad before.



You can save some time by downloading my Orcad project file for a single driver unit, just change the RLC values and you can start trying OrCad simulation right away.



Let's do the woofer as an example. First, start up Orcad Capture and create a new empty project. Then in the schematic draw the driver model using Place->Part... command. The R, L and C are all under the ANALOG library. (You may need to add all libraries first if you have not done it.) Then add the AC voltage source (called VAC under the SOURCE lib.) and also add a ground reference by Place -> Ground... -> 0/Source. Connect all components by Place->Wire. You should now have a circuit similar to the one below :


Let's do some simulation: Add a new simulation profile by select PSpice-> New Simulation Profile, type in a name. A simulation settings dialog will pop up. In the Analysis tab, set Analysis type to AC Sweep/Noise. Select Logarithmic, start frequency of 10Hz, End Frequency of 20kHz, Points/Decade to 50. Click OK.


Now place a voltage probe and a current probe at input of the of the resistor, by selecting PSpice -> Markers -> Voltage Level, and then point the probe at the line between the VAC and the resistor. Select PSpice -> Markers -> Current into Pin, and select the input pin of the resistor.


Select PSpice -> Run to start simulation. After the simulation is done, the result will pop up in another PSpice A/D window. Now you can see the voltage and current that go into the driver at different frequency. To get a impedance plot, you have to add a trace, by selecting Trace -> Add Trace, then type V(V2:+)/I(R1) in the Trace Expression input line, then OK. Now you should see the driver unit's impedance vs frequency, like the one below.


You can compare the result to the impedance plot from the driver unit's datasheet, or better yet, compare it to your measured impedance. If they look similar, then this should be a good model to use, if not, tune your circuit's RLC value until they are close enough.


Page 1 of 2


>> NEXT Page : Crossover + Drivers Simulation




Privacy Policies | Site Map | Contact Us |