Welcome to Solid State Guitar Amp Forum | DIY Guitar Amplifiers. Please login or sign up.

March 28, 2024, 01:41:37 PM

Login with username, password and session length

Recent Posts

 

Ashdown peacemaker 40 schematic reading problems

Started by Stormlord1736, October 18, 2014, 10:47:12 AM

Previous topic - Next topic

Stormlord1736

Hello,
I have some doubt about the schematic of this amplifier, I attach the file.

My purpose is not to physically build this amp (since I have the original at home). I'm studying about amp modeling, so I want to simulate it.
First of all I need to copy the amp schematic on spice, in order to make a comparison between the model and the real amp.

So, these are my questions:

1)
First of all, I want to ask about power supply circuit that generate DC voltage for the tube.
It is placed in file b in the bottom right.
Blue-1 and Blue-2 represent the power socket right?
I have a doubt about the inscription "AC IN 270", what is 270? It's the effective value or the peak value?

However, I implemented this circuit in spice using 50Hz 270V sine input, in other to find CT, G2, HT1, HT2 and HT3. The problem is that I get the same DC output voltage for each of them, I don't think that this is the correct result, what do you think about that?

2)
The second question is about the Belton Reverb always located in the file b. I think it is a spring reverb, but how can I model it on spice? in other searching on google that brand/model did not find any results.

3)
The last question is about ouput transformer, it can be found in file a. I don't fully understand the meaning of the "ring symbol" for which a color is indicated (ex. BLUE YELL WHITE BLACK ecc), what do they represent?.
In addition to model accurately the transformer I should know the brand/model in other to know the material and the non-linear relationships.
From this schematic how can I know what type of transformer is that? how can I get its model?
Since that I have the physical amplifier at home maybe I can see the model dismounting it?

Thanks in advance for any replies.


g1

  The 270V is the RMS value of the AC voltage coming out of the power transformer.
If you have not simulated the whole circuit, you will not see the proper voltages.
With no loads on the various points in the power supply, they will all show the same voltage when simulated, as you have found.
The belton tank is the equivalent of an accutronics model 8EA1C1B.
The colors shown for the output transformer are the wires connected to it.
You may find a model number on the output transformer itself, but that will probably not get you anywhere.
For proper simulation of the OT you will probably need some spec like the turns ratio or input and output impedance.
Others here that use spice may have better ideas, I have never used it.

Roly

Hi Stormlord1736, welcome.


Quote from: Stormlord17362)
The second question is about the Belton Reverb always located in the file b. I think it is a spring reverb, but how can I model it on spice?

Unless you want to get neck deep, as a simple transformer represented by the resistance and inductance of the line driver and receiver, where you will get signal but no reverb delay. {If you really want to simulate a reverb springline then you will need to model it as a transmission line, but there is seldom any need to go to those lengths.}

Quote from: Stormlord1736I don't fully understand the meaning of the "ring symbol" for which a color is indicated (ex. BLUE YELL WHITE BLACK ecc), what do they represent?.

In addition to model accurately the transformer I should know the brand/model in other to know the material and the non-linear relationships.

They represent the drafts-person being lazy.  The left hand trio are the output transformer primary, end - center-tap - end.  The right hand quad are the secondary winding, common and three impedance tappings.


In LTSpice you specify the inductance of each transformer winding and this gives the sim the turns ratio (you can include the winding resistance but this is normally insignificant).  You also have to specify the coupling index between the windings which is specified using the statement "K1 L1 L2 L3 L4 L5 0.9" where K is the coupling factor shared by the individual windings L1 - L5, value 0.9 (typical guess).  L1 and L2 will be the primary, and again you can generally treat the secondary as a single inductance of the winding in use, e.g. 8 ohms.

Since you have one of these amps to hand the easy path is to measure the inductances (unless you can find a spec sheet that gives them - possible but unlikely).

HTH

If you say theory and practice don't agree you haven't applied enough theory.

Stormlord1736

Tnx, for the answare. I have a few more questions.

Quote from: g1
The belton tank is the equivalent of an accutronics model 8EA1C1B.
On the accutronics website I only found the 8EA2C1B, it's the same?

Quote from: Roly
Unless you want to get neck deep, as a simple transformer represented by the resistance and inductance of the line driver and receiver, where you will get signal but no reverb delay. {If you really want to simulate a reverb springline then you will need to model it as a transmission line, but there is seldom any need to go to those lengths.}
For the moment I'm only interested in simulating its behavior when the reverb knob is at 0. It's just a impedance? Or there are also some non-linearity or other behaviors to be simulated?


At the moment I realized the circuit on spice bypassing the reverb/effects part and I used this transformer model:

.SUBCKT OutXFMR_10k:8 1 2 3 4
L1 1 5 200H
R1 5 2300
L2 3 6 .16H
4 .2 6 R2
K1 L1 L2 .99996
C1 1 5p 5
C2 3 6 20p
C3 5 6 200p
.ENDS

I don't know what should be the input impedance. So the 10k value was chosen randomly.

Since I am not practical, I would like to know if there are any errors in the circuit that I wrote. Surely the CT voltage is placed in the wrong way, but I haven't understood how to place it.

Here the images from spice circuit:
https://www.dropbox.com/s/6ul6o3s4crgm9jd/peacemaker%2040%20spice.pdf?dl=0

Regarding the power supply circuit, I'm having trouble in transient simulation since the CT, G2, HT1, HT2, HT3 voltages take a long time to get up to steady state and the simulation time become too long.
I would like to replace these volteges with ideal generators, but first I need to know the right value, how can I do this?

Thanks in advance for any replies.

teemuk

#4
QuoteHT3 voltages take a long time to get up to steady state and the simulation time become too long.
I would like to replace these volteges with ideal generators, but first I need to know the right value, how can I do this?

There are several options to overcome the particular issue:

1) Run the simulation for enough time for all DC voltages to "settle". Use those values for ideal voltage sources. Usually you only need just one or two DC sources because with DC voltage sources in the supply the solver doesn't have to plot the time it takes for all capacitors to get charged by the pulsating DC.

Naturally the rectified AC voltage source will fluctuate according to current draw while the "ideal" DC voltage source won't. One of compromises between simulation speed vs. simulation accuracy. This also introduces an issue whether you want to derive and use "unloaded" or "loaded" supply voltages, which will be somewhat different.

2) Introduce a time delay for "plotting". For example, LTSpice transient analysis has the "time to start saving data" option. This option can be used for the plotter to skip over the period that it takes for voltages to settle. The solver will run but it won't plot anything, so it's a tad bit faster that way. If you also "mute" the input for this time (put a delay to input signal source as well) the voltages will settle faster as the circuit runs "unloaded" for a moment and draws less current.

3) I don't remember the SPICE directives from top of my head but refer to very good built-in "Help" documentation. There is an option that allows saving all circuit voltages at given time of simulation to an external file, and then restoring them from this file for new simulations. This way you only have to run the "voltage settling" period of simulation only once. Later you simply restore the voltage condition from file and rest of the simulation runs to end from that point. Much, much, much faster....

I use this method if I really want to include effects of rectified and fluctuating power supply to the simulation. It's not always that important but can make simulations of say, tube power amps, more realistic since effects of voltage sag and such are included. If you use an external audio file as input signal source and include a rectified power supply simulation then doing this is pretty much a "must". ...unless you want to start adding those muted periods in the beginning of each waveform. I prefer not to, not to mention the far greater speed to run the simulation.

The drawback is that if you make any bigger modifications to circuit you'll have to run the initial "solver" again to get results that match the modified circuit.

g1

Quote from: Stormlord1736 on October 24, 2014, 05:10:49 PM
Tnx, for the answare. I have a few more questions.

Quote from: g1
The belton tank is the equivalent of an accutronics model 8EA1C1B.
On the accutronics website I only found the 8EA2C1B, it's the same?
The fourth digit denotes the delay length.  The 1 is short delay, 2 is medium.
Otherwise the specs are the same.
The codes are explained on this page:
https://www.amplifiedparts.com/tech_corner/spring_reverb_tanks_explained_and_compared

Stormlord1736

#6
Quote from: teemuk
There are several options to overcome the particular issue:
Yes thanks, my bad. Obviously with an high frequency input signal the simulation integration step must be much smaller.
So, I've done a simulation of 20 seconds by placing the input to 0V and then I took the voltage values. I used the command ".ic v (node) = value" to set initial condition, in orther to get faster the steady state.

Here the new version of the spice schematic:
https://www.dropbox.com/s/r9xfff70h5t39b9/peacemaker%2040%20spice.png?dl=0

I also understood how to connect the CT voltage. Reguarding the inductance values, I took them from another schematic, but I don't think they are also suitable for this circuit.
1) How can I get the correct values for this amplifier?

The final output signal is near to be a square wave, I think it's too distorted to be a clean channel.
2) Where I can find in the schematic, the potentiometer for power amp volume?

In addition, the value of CT fluctuate, more less, between 342V and 300V.
3) It's normal, or it's too much?


Thanks in advance for any replies.

Roly

Quote from: Stormlord1736the inductance values, I took them from another schematic, but I don't think they are also suitable for this circuit.
1) How can I get the correct values for this amplifier?

The inductance (impedance) ratio looks far too high.

A pair of 6BQ5's in push-pull require 8k plate-to-plate, so a quad requires about 4k p-p, which is 1k either side of the centre tap.

1000/8 = 125:1
125 * 0.3 = 37.5H each side of the primary.

You will find a potentiometer symbol and associated sub file at Yahoo Groups LTSpice Group.
If you say theory and practice don't agree you haven't applied enough theory.

Stormlord1736

#8
QuoteThe inductance (impedance) ratio looks far too high.

A pair of 6BQ5's in push-pull require 8k plate-to-plate, so a quad requires about 4k p-p, which is 1k either side of the centre tap.

1000/8 = 125:1
125 * 0.3 = 37.5H each side of the primary.
Ok, thanks.

QuoteYou will find a potentiometer symbol and associated sub file at Yahoo Groups LTSpice Group.
I'm sorry I explained badly, I write better the question.
From the schematic I found only 6 knobs:
Channel 1: Gain, Treble, Middle, Bass, Volume
Channel 2/3: Gain, Treble, Middle, Bass, Volume

I hope I identified them correctly. The problem is that I can't find from the schematic this knobs: Reverb, Volume 1 and Volume 2.

Here are pictures of the amplifier and knobs shown on the schematic:
https://www.dropbox.com/s/9xidsnorwh3o8pg/peacemaker%2040%20images.pdf?dl=0

Thanks in advance for any replies.

g1

  You posted 2 schematics, look at the other one for masters and reverb.
I guess there is a FX level pot also on the back of unit?

Stormlord1736

#10
Quote from: g1
You posted 2 schematics, look at the other one for masters and reverb.

Ok, I found master and reverb knob thanks.

Quote from: g1
I guess there is a FX level pot also on the back of unit?

Yes, I have effects send/return and knob for effect mix.

I have a few more questions:
1) In the schematic a in the preamp circuit there is C15 but instead of the value is written Ɔ/C what it mean?
2) In the schematic b there are A1 and A2, I must consider them linked together?
3) In the schematic a there is TP1 10V, what is it? where is it connected?
4) In the schematic b, the circtuit on the bottom left with AC IN. What is it? What is it for? What are the components IC4: 7812 and IC5: 7912?
5) In the schematic a/b there is a node called: Boost LD, that comes from input jack RNB - BOOST... But I don't have this jack on the back of the amp (attached the image to this post). Where it should be this input jack? what is it?


Thanks in advance for any replies.

Roly

Quote from: Stormlord1736I have a few more questions:
1) In the schematic a in the preamp circuit there is C15 but instead of the value is written ?/C what it mean?
2) In the schematic b there are A1 and A2, I must consider them linked together?
3) In the schematic a there is TP1 10V, what is it? where is it connected?
4) In the schematic b, the circtuit on the bottom left with AC IN. What is it? What is it for? What are the components IC4: 7812 and IC5: 7912?
5) In the schematic a/b there is a node called: Boost LD, that comes from input jack RNB - BOOST... But I don't have this jack on the back of the amp (attached the image to this post). Where it should be this input jack? what is it?

1. "o/c" = open circuit, i.e. shown on the circuit but not actually fitted in production.  There will be a place for it on the board, but it will be empty.

2. These concentric circles are a non-standard symbol but, given the context around the output transformer, they appear to be termination points for wiring that is off the printed circuit board.  TR4, MPSA42, is a 300 volt transistor, so I expect that you will find an off-board wire connection between points "A1" and "A2" (which should be marked somewhere on the board overprint).

3. TP1 is "Test Point 1" and is used to measure the cathode voltage across R61 as a proxy for the total cathode current (100 ohms means 0.1V per mA) when checking the output stage standing bias.  It should be 10 volts, meaning a total current of 100mA for the four valves.  Test Points are not normally connected to anything (other than your meter during servicing).

4. This is the low voltage power supply for the preamp section.  It produces two regulated voltage of +12VDC and -12VDC.  IC's 4 and 5, 7812 and 7912, are three-pin 12 volt voltage regulators, one +ve, the other -ve.  (Diodes D8 and D9 are to bump this voltage up slightly to the +/-12.8V value shown.)  The "AC IN" is 30VAC centre-tapped (i.e. 15-0-15 VAC) from the power transformer.

5. Socket SK7 (circuit b) is for the multi-function foot pedal, one of the functions of which is "Boost".  This boost request goes to the output arrow BOOST_LD (cct b) which is the same point as the input arrow BOOST_LD on circuit a.  This switches the FET TR3 which is across R43.  When this FET is switched on it causes the gain of the V5a stage to be increased ("boosted").

The designation next to SK7 is actually "Ring = Boost, Tip = Ch1/2".  On 6.5mm (1/4-inch) "stereo" plugs the three connections are the body for ground, the tip contact, and the ring contact, hence these are sometimes called "TRS" for Tip-Ring-Sleeve.  The footswitch connected to the tip controls the channel switching, and the footswitch connected to the ring controls the boost function.



HTH

If you say theory and practice don't agree you haven't applied enough theory.

J M Fahey

Simulation is a great tool, but to simulate the entire amp, you need models for every single part, and very much doubt you can them for the ëlectromechanical:  parts such as speakers, transformers and reverb tanks.

Of course, someday, somebody will model and publish them all, but so far I think the sensible use is to simulate *parts* n of the circuit, such as how the preamp distorts, how tone controls work, etc.

But for the full all-at-once picture, you'll always miss some tiny bit here and there.

phatt

Quote from: J M Fahey on November 12, 2014, 06:32:21 AM
Simulation is a great tool, but to simulate the entire amp, you need models for every single part, and very much doubt you can them for the ëlectromechanical:  parts such as speakers, transformers and reverb tanks.

Of course, someday, somebody will model and publish them all, but so far I think the sensible use is to simulate *parts* n of the circuit, such as how the preamp distorts, how tone controls work, etc.

But for the full all-at-once picture, you'll always miss some tiny bit here and there.

Wise words.  :dbtu:
Reminds me of those 65 deluxe reverb pedals claiming the sonic signature of the original amp,, I'm dying to know how one could possibly replicate tank slap which is the tiny magnet hitting the iron core, a purely mechanical action. xP
Phil.

Roly

The same thing, but from a slightly different angle - the ultimate simulation is to build the actual circuit.  This includes all the off-circuit stuff like stray capacitances and inductances, and minor n-th order stuff left out of simulation models.

You get to a point where real components are easier to obtain than realistic models and it becomes easier to "throw it up against the universe and see what sticks" than continuing to hibber in the theoretical - and it's totally realistic.

It is possible (and there is a natural inclination) to go on refining a design well past the point where it needs to be tested in reality, an actual prototype build, which will often throw up things the sim won't.

LTSpice is a fantastic tool, but it has its practical limits.
If you say theory and practice don't agree you haven't applied enough theory.