The 'Tater Patch

[Robert McLean]

Valveitude :

Just how accurate is spice at predicting "real world" performance? I suspect it boils down to the accuracy of the tube model.

Your tube model is using Koren's equations, and I have found it to be pretty good, so your tube model probably should be OK.

But there are 2 other factors that can affect the reality of distortion indicated by spice.

The first is the transformer. Your transformer model is not very realistic in that it has no resistance, or capacitance, or core saturation effects. The first 2 mean frequency response will not be correct, and the second means distortion will not be correct. There are several ways to model the resistance and capacitance, but I do not know how to model the core saturation effects, but I believe there are ways. But of course you can still use your model to compare changes in the tube circuitry.

The second thing to look out for with respect to harmonics with spice is the minimum time step used when you run the transient analysis. I only mention this since you state this is your first time spiceing something. You may already know this. But to prove it to yourself enter a spice circuit consisting of a sine wave voltage source at say 1000 Hz, and a resistor load. Put in a Four statement. Run the simulation and you will find that although you should in reality get 0 distortion, since it is pure sine wave source, LTSpice gives you lots of distortion unless the maximum time step specified is small enough. What I do is take the period of the source and divide by 16384 for accurate runs, and by 2048 for quicker runs. So that I dont have to recalculate stuff every time I change frequencies, I use the following set of parameters in and include file :

;**** declarations for transient analysis
; param Freq is declared on the main schematic
.param Period = 1 / {Freq}
.param Period2 = 2 / {Freq} ; 2 periods
.param Period3 = 3 / {Freq} ; 3 periods
.param Period4 = 4 / {Freq} ; 4 periods
.param HPoints = 16384 ; power of 2 for most accurate fourier analysis
.param HTmax = 1/ ( {Freq} * {HPoints} ) ; maximum time step for best fourier analysis
.param Points = 2048 ; number of points per period for other runs
.param Tmax = 1/( {Freq} * {Points} ) ; maximum time step for other runs
.param HalfP = 0.5 / {Freq} ; half a period, for square waves
.param Trise = 1 / ( {Freq} * 1000 ) ; rise time for square waves, also fall time

I then use the parameters in my circuit rather than numbers.

[valveitude]

The input capacitance of your proposed amplifier will be rather large to say the least...

I guess roughly 350-450pF

I'm confoozid...wouldn't that value range shunted by 33.3k (100k/3) indicate a roll-off between 10kz-15kz ? My simulation shows considerably more extension than that. What am I missing here? Truth be told, I selected the grid resistors based on this circuit , as it seemed to be the "optimistic" choice. I may lower it.

Does the input capacitance effect more than the frequency
response ?

P.S. I can sleep easier Sy knowing your extreme makeover has seemed to be a success. Your old avatar was giving me the willie's ( I suppose that was the point )

[valveitude]

Your tube model is using Koren's equations, and I have found it to be pretty good, so your tube model probably should be OK.

Good to hear

But there are 2 other factors that can affect the reality of distortion indicated by spice.

The first is the transformer. Your transformer model is not very realistic in that it has no resistance, or capacitance, or core saturation effects.

Yah, I know. Since I will be winding it myself, I don't have any "real" numbers to go by. I figure that it will be the limiting factor in the actual amp, and its performance compared to the projection will tell me how well I did winding it.

There are several ways to model the resistance and capacitance

Which method would you suggest ?

The second thing to look out for with respect to harmonics with spice is the minimum time step used when you run the transient analysis. I only mention this since you state this is your first time spiceing something. You may already know this.

I found this out the hard way. After getting some screwy results, I searched this forum and learned about the time step thingy, I also saw that the sample window needs to be divisible by the freq., ie, a 12 ms sample for 1k.

So that I dont have to recalculate stuff every time I change frequencies, I use the following set of parameters in and include file :

Egg-suh-lent!!! I WILL play with that. How do you toggle between fast/accurate ?

Casey

[valveitude]

You refute my amp comments well. It does not suit me but it may suit you fine.

Well, it is all about me...ME,ME,ME !!

I am astounded that you can get 5,000-10,000 Gauss across a 1/2" or even 3/4" gap, a yard long, with chump-change magnets.

I am too. I played around with ribbons years ago and never got close to this.

A couple times in that thread, a concise list of equations for efficiency and sensitivity were posted. They seem to take no account of air loading. This is an acceptable assumption for the original treble-only drivers. It can't be neglected at 100Hz on a 36"x0.75" radiator.

Well, I think my ribbon more closely approximates 1.5"x 36" (two .75" ribbons side by side). As far as the low end roll-off, 100hz is my "blue sky's" design point. If I can't get down to 100hz with 54 sq. in. of radiator surface, I'll either raise my x-over point to suit, or use up some of my efficiency with a passive eq. Either way I "think" I can get what I'm after.

Casey

[SY]

The RC time constant you need to look at is the source impedance of the circuit driving the Spud with the Spud's input capacitance. Then verify that the source has the capability to source enough current to drive that capacitance to whatever is the required voltage at the highest desired frequency.

Dirch Passer will only be grinning at you until I find an even ookier avatar. The search continues...

[valveitude]

The RC time constant you need to look at is the source impedance of the circuit driving the Spud with the Spud's input capacitance. Then verify that the source has the capability to source enough current to drive that capacitance to whatever is the required voltage at the highest desired frequency.

Gotcha..thanx. Putting 5k of resistance in series with the source dropped the 20khz response .5 dB. The whole system is starting from scratch, looks like I'll need to ensure my source impedance doesn't drop below 5k, preferably 1K.

Dirch Passer will only be grinning at you until I find an even ookier avatar. The search continues...

Oh goody...can't wait.

[valveitude]

The whole system is starting from scratch, looks like I'll need to ensure my source impedance doesn't drop below 5k, preferably 1K.

Uhh..that should be "doesn't rise above 5K"..think I'll go snif some more glue.

[Robert McLean]

Valvitude :

quote:
There are several ways to model the resistance and capacitance

Which method would you suggest ?

I use the following type of model. It can be expanded to do push pull, and ultralinear, and multiple outputs.


.SUBCKT 5KSE P1 P2 Sp1 Sp2
* Single ended audio transformer
* 5k to 8 ohm, 10 to 40KHz
*
LP1 1 P2 40.26021568H ; PRIMARY
LSA 2 Sp2 0.064416345H ; SPEAKER SECONDARY
KALL LP1 LSA 0.999499875 ;
RP1 P1 1 56
RS Sp1 2 .1
.ENDS

Basically you can set the 3 dB points by varying the coupling factor. So if the 3db points are specified, you can calculate the required coupling factor. I have the eqautions somewhere, but I am having trouble finding them. Basically they are the equations for broadband transformer coupling. I have a spread sheet I use for the calculations.

Now the model is not totally realistic, but at least it gives an upper and lower frequency roll off. I have tried other models based on a leakage inductance combined with a transformer with K =1, but I found these gave trouble in some circuits for some reason.




quote:
So that I dont have to recalculate stuff every time I change frequencies, I use the following set of parameters in and include file :

Egg-suh-lent!!! I WILL play with that. How do you toggle between fast/accurate ?


In the transient dialog box I just enter the parameter names rather than values ie for the full accuracy run
for Stop Time enter {Period2}
for Start Time enter {Period}
for Maximum Timestep enter {hTMax}

I start at {Period} rather than 0 to give the circuit time to settle down a bit.

for a quick check I do
Stop Time {Period}
Start Time 0
Maximum Timestep {TMax}

and of course on the schematic I have the statements
.inc MyLibs.inc (which contains those equations, and other stuff )
.param Freq = 1k (or whatever I want )

and in my voltage source and Four statement I put {Freq} wherever a frequency is called for.