Crystal Filter Design

i can only draw and simulate in spice way .all the same

please help in this, how to simulate? how u calculated those values

There are plenty of companies that produce such thing, hunt out one on the internet why try to redevelop the wheel ?

For that bandwidth and centre frequency your design will almost certainly need custom designed crystals.

To be able to specify the design parameters to the crystal manufacturers you will need to know how to design crystals... Not an easy task...

I know I've designed a crystal if filter for a Marconi spectrum analyser...

If you want my advice either do as the previous poster said and get someone else to design and manufacture it, or find another way out of using crystals!

John.

As folks here have said this is not a trivial task I know I do it for a living. SPICE dosn't help design anything it merely tests a model of what you think you have.

My advice is to hire an expert if this is a job, or get some refeence designs that do work and try to reverse engineer them for your application.

If your just tinkering in the lab and curious about Crystal Filter design look on the web and do a google search on the subject.

The advice of Wm Stutz's cat is excellent, but watch out - most (?all) web articles don't contain enough information to enable you to design a good quality filter.

I'd add another caution: if you are going to do transient analysis of systems that incorporate the filter, PSPICE is probably not the correct tool. The speciifc problem with PSPICE is that, in transient simulation, it uses the Gear2 integration algorithm exclusively - and this has the charactersitic of showing a simulated Q that is lower than the actual circuit will exhibit. Use almost any other SPICE-like simulator - provided you can be sure that it uses trapezoidal integration algorithm for transients. LTSpice is one of the more robust, and it is available free from the web.

Back to the filter design itself: the level of difficulty depends on what you need to achieve. If you just want to design a first or second order filter so as to attain a first-order understanding of what crystal filters might look like, you only need to use the data-sheet model of the crystals (C0, C1, R1). You can then either resonate out the parallel capacitance C0, or (much better) build a transformer bridge to suppress the effect over a wider bandwidth. From there on, you can design the filter based on standard filter design methods.

Now to warn you what you might be letting yourself in for if you wish to design for real performance:

The first real difficulty of crystal filter design is that the published resonance is just one of many "inharmonics" that are present in a frequency region that is quite close above the nominal frequency (this is in addition to overtones - which, be warned, are not exact multiples). This isn't too much of a problem for most use in oscillators, as these inharmonics are more lossy than the wanted mode. However, the loss you introduce when broadening the bandwidth for filter use means that the relative breakthrough at the inharmonic resonance frequencies can become very significant. The solution generally adopted is to use crystals with different characteristics* (and so different frequency inharmonics) in a configuration that allows one filter to suppress the inharmonic of another. For this, you need access to the process.
*Either different designs, or selection of crystals that required different amount of adjustment in manufacture.

Another issue that you are unlikely to be able to control unless you are working closely with a crystal manufacturer is intermodulation distortion. First, there is the intrinsic distortion due to quartz nonlinearity - this is minimised by matching the acoustic strain amplitudes within the filter (depending on specification details, parallel stagger-tuned designs can also be helpful). Then there are the effects of manufacturing "imperfections" - low (by most standards) levels of surface contamination, lack of electrode adhesion, interactions with mountings and adhesives can all play a part here.

Another "feature" is microphony. Filters have lower signal levels than oscillators, and so are more susceptible to "direct" acoustic coupling - although this tends to be more of a problem at lower frequencies). But the resonance-frequency of crystals is acceleration sensitive, and this can be an issue in generating side-tones.

Finally for this contribution, and of particular significance in narrow-band and high-order filters: mismatch between the temperature coefficients of the crystal components can distort the passband away from the nominal temperature.

Good luck

It all depends on the degree of performance you wish to achive, if you just want to improve the performance of a telegraphy or facimile radio reciever a simple one or two pole device which is very easy to design may well surfice but if you want a really flat pass band and very steep flanks and no spurious responces it is a job for the professionals

Hi Syphrum - I think you are agreeing with my: "Back to the filter design itself: the level of difficulty depends on what you need to achieve", but it didn't quite read like that.
Returning to the design of the filter: if it was to be a two-pole filter, and there was any possibility of operating the filter at a standard filter frequency, I think I would calculate the coupling coeffcieint needed for the response I want, and select the nearest available (standard) two-pole monolithic crystal. Manufacturers will usually provide motional parameters if asked. I would then load it to provide the closest response practical. That way, you should be able to guarantee that the inharmonics have been catered for. (You could in principle modify the coupling by using a reactor in the ground pin of the monolithic crystal, but that would of course degrade the stopband rejection). The advantage of this approach is that, if you eventually need a good number of parts, the manufacturer should be able to provide a monolithic crystal with the coupling coefficient that you really require - and without any retooling being necessary.

Physicist has enumerated the depth of the problem quite well and my cat was impressed! His comment regarding SPICE simulation is well taken, "Know your tools".

For that reason I use MathCad where I can select Romberg Trapezoidal approximation with Richard extrapolation, among other things . For actual simulations (SPICE) I use a low cost program called Beige Bag thats a SPICE3 engine (Written in C) not the old Fortran stuff and you can find it on the web as www.beigebag.com

It allows you to make or import CADSTAR models if you want and will give you better results I think.

If you already have a SPICE simulator try using the .OPTIONS statement. If you choose the

.OPTIONS METHOD=GEAR you get the GEAR-2 method but if you use the

.OPTIONS METHOD=TRAP you'll get the trapazoidal method (recommended).

You can also use the backward Euler method if you chose the (undocuemented in SPICE2) MU option which is why I prefer SPICE3. The way this works is to choose

.OPTIONS MU= X

When x=0 you get the Euler method, if MU 0.5 you get the trapazoidal method, and 0>X> 0.5 you get a blend of the two.

Trapazoidal integration may also contribute errors! One of the well known ones is "Trapazoidal Oscillation", (TO) and another is "Error Accumulation" (EA).

TO results from too large a step size in the simulation and the results will seem to "oscillate" about a value while EA introduces small errors which accumulate during intergration. While the Euler method doesn't exhibit TO it will exhibit EA errors.

For this reason I vary the value of X and look at the results. EA will give results that appear to defy the laws of Physics!!!

Well I seem to have left the thread of this which was crystal filter design and I apoligize for that but it simply points out all the pitfalls one faces in doing such a design (I think).

One thing that runs through all of this is the fact that you need a crystal that matches the assumptions you have in the model. I spend alot of time measuring parts to make sure that is so. This requires a good synthesizer with very low harmonic distortion and alot of patience.

One aspect I didn't see mentioned was the circuit should be embedded in a "Roofing Filter" to reject the harmonic responses that inevitably result. I usually try to include this in the impedance matching circuitry. A tapped tank circuit works well for this and improves the overall response of the circuit.

Bill S

I am a technician not an engineer, I would wind a small coil tuned with a capacitor to 10MHz with an auxiliary winding to provide a low impedance bi phase output.

Buy a couple of crystals 10MHz series resonant plus/minus 750 Hz feed one phase into each and take the common output to a variable resitor of about 500 ohms.

Construct a simple swept oscillator swept by the horizontal scan of your oscilloscope, Feed this into your transformer and look at the output at the resistor, adjust the resistor until the peak is fairly level , if the bandwidth is too wide try a pair of crystals slightly closer to 10MHz, this is the sort of system used in communication radios from about 1920 to 1980

Its called designing with a soldering iron.

It's also called a two-pole lattice, and this is a reasonable way to implement one. It provides the two variables you require (frequency spacing and load impedance). But you probably need to have crystals of similar C1 (and therefore similar type type) to Syphrum's if a load near 500-Ohm load is to be correct for a 2-kHz bandwidth.

Thank you Bill Stutz for your notes. The point about needing a roofing filter was well made.

The remainder of this is about tools: I have a question about Mathcad, and and some additional information for SPICE users:

Mathcad is OK, but I used to have personal problems with the interface. Is a more equation-based version available now?

Next, some notes about integration algorithms (warnings for the innocent?).
For those who might try it without appreciationg the benefit/risks: backward Euler gives the most reliable numerical convergence of any of the straightforward integration algorithms. The downside is that it damps the apparent Q of any resonance by a greater amount than any of the other algorithms. It is the standard algorithm used for establishing DC conditions, because in this case all that matters is to get a sensible solution. Backward Euler is also used in SPECTRE to rescue transient simulations that "get into trouble"; but it is only used for a short time period, and at least you get a warning..
Next, "Trapezoidal Oscillation" this so-called oscillation is the result of truncating each successive approximation when it has reached the accuracy you specify. So if you set the truncation limits (PSICE calls these "tolerances") too loose for your application, you will see an error that alternates on either side of the 'proper' local solution. In fact, this alternation of the error is directly related to the reason that TRAP does not cause systematic cumulative damping. Gear2 and backward-Euler both leave truncation errors on the damped side of the proper solution. This makes them look prettier when you are looking at the limits of the tolerances, but the dleetorious effects of the errors can be much larger.
I believe that what you identify as Error Accumulation (it's not a term I use in this context) in Trapezoidal Integration is a consequence of the random nature of the errors. Realistically, this only occurs in circuits that are effectively neutral over the simulation period - to that extent, it mimics what would actually happen if the noise level in the "real" system was equal to the truncation error ofthe simulator. It can be reduced by tightening the simulation tolerances. (But don't take this too far, because it makes he simulation run slower - and you can cause it to fail if numerical noise exceeds the test levels)
While on this subject, TRAP does also cause systematic errors - but they affect circuit time-evolution/frequency, not Q. For most filters, Q-errors are more difficult to handle - provided that the time/frequency errors in different parts of the circuit are of similar magnitude. (Essentially, the effect on the stability depends on the lowest polynomial order for which the algorithm produces errors. Trapezoid is the lowest-order stability-maintaining algorithm, and the only one implemented in SPICE)

In spite of its weird extended name, I recommend you take a look at LTspice - some reasons below:

I used Beigebag many moons ago. In those days it was a recompilation of plain Berkeley SPICE3. So far as I know, it still is - although it may have some additional bells and whistles. The basic principle behind LTSpice (as behind any other usable premium versions - e.g.SIMetrix, ELDO, SPECTRE) is the same as SPICE. What they improve are the matrix solving methods, the stepping algorithms, the numeric algorithms (yes, that is possible too), etc.. Special models can also help. With one exception (= no pseudotransient for DC solution), LTSPice is as good as any, and, as I said free. It also provides Laplace, and implements lossy reactors with just two nodes (this is in itself an advantage, but the associated change in methodology gives further benefits). LTSPice also has quite a few other bells and whistles, but these may take a bit of learning. However, you can run it direct from most 'standard' forms of netlist (including HSPICE, and I think LT may have added PSPICE). Unfortunately, you lose LTSPices (extensive) range of probing tools when you do this, but it can give a standard SPICE output for use with your existing tools. N.B. that LTSpice works (correctly) without problems on many circuits that give problems in Berkeley-SPICE3, and in PSPICE.

hi

where can i get the data sheets that gives the values of C0, C1, R1, to build the crytsal filter for 10 Mhz, i searched in the internet , i didn't find any,

please help me in this.

Thanks

C1 is not generally specified in general data sheets, except where the data sheet only covers a specific frequency (and not always then). The basic reason is that these crystals are mostly intended for oscillator use, and C1 varies somewhat chaotically with frequency (its value is determined by the need to avoid activity dips and other manufacturing considerations)

In the end, you will need to talk to the manufacturer. Fortunately, they are used to this.

For very rough guidance only (and to give you something to set up your simulations) you might expect a 10-MHz crystal in an (old-style?) HC49 package to have C0 ~ 2.5-pF, C1 ~ 8-fF, and R1 between 6 and 30 Ohms. There will be capacitance between each of the pins and the package; to minimise crosstalk and pickup, you will probably wish to ground the package.

An additional word of warning - crystals that are designed for use in fixed-frequency oscillators can show excursions in their properties at specific temperatures - so an otherwise well-designed filter might not work as expected at these temperatures.

Manufacturers may find it easier to match your needs if you can use a standard crystal filter frequency such as 10.7-MHz; this again is a case for talking to them.

Application notes for simulation of oscillators may be of limited help - e.g.

Good luck

fyz

PS for anyone designing oscillators: the above article quotes the Barkhausen criterion, but it is dangerous to use this, as it only provides the low-gain limit. For crystal oscillators the presence of C0 means that there is also a high gain limit. Safer methods include full Nyquist plots and (more pragmatically) modelling the negative resistance between the crystal terminals (C0 must be present in the simulation)

Zverev has tables of design parameters for cook-book crystal filters as well as methods. It was written in pre-simulation days, though. Also covers basic filter responses (I recall Chebyshev, Bessel, various transitional types) but you haven't mentioned any phase requirements.

Handbook of Filter Synthesis by Anatol I. Zverev (Author). Sort of pricey, but a good reference. I've kept a copy about since about 1984. As I get older and lose brain cells I can still use the tables, though lately the commentary has made me squint.

So that's where my copy went...

Seriously, though, there's quite a lot of front-end effort required before you can use Zverev, and it doesn't provide any guidance with the second order effects discussed by wmstutz and Physicist. If Anonymous is designing a simple filter he's almost certainly better off without it

If Anonymous already has some crystals he wants to try, the best thing would be to measure the 3-dB bandwidth with a range of resistors placed in series with botht he source and the crystal. From this he could readily calculate both C1 and R1. C0 readily follows from the parallel resonance frequency.

He may even be able to select crystals with staggered inharmonics and/or overtones to use together to maximise out-of-band rejection - though the ultimate performance is likely to be better if his crystals are to difference C1 specifications or come from different sources.

(All this is far too late of course - just added for completeness)