Siemens W295b

Hello you DIY guys! 

First of all, since this is my first post here, I wanted to introduce myself. My name is Phillip, I'm from Germany, I have a "Diplom" in Engineering Physics, but not really a clue when it comes to electonics 
I started to get interested in audio equipment during the first recordings with my band in the last years and because I tend to get lost in details I eventually stranded here in the forum.
In the last couple of month I started building audio equipment on my own. My first amplifier (based on the Silver Elements Kit by Hairballaudio) should be ready by next week, so I am looking for my next challange.  8)

In order to create my own channel strip eventually I decided to build an EQ next, and because I really like the sound of the Soundtoys "Sie-Q" VST plugin I am very interested in the "Siemens W295b" EQ.

Instead of buing some old crap from ebay and trying to refurbish it, I decided to take a look at the schematics and try to understand what's going on in there first.

Based on the schematic attached I started modeling the circuit in LTSpice, using modern transistors similar to those in the schematic but still available. The input stage of my simulation does as it should do, but the following RC-Network  for bass and treble control does some nasty stuff to the frequency response.

I will attach the schematic of my simulation in the next post.

Can you explain to me what the RC-network is doing exactly?

It is not a classic Baxandall network, is it?

Why are there two outputs feeding the following stage?

Can you spot any mistakes in the simulated circuit? (Junction in a place where there shouldn't be one etc.)

Thanks in advance! 

Phillip

Here's the simulation schmatic. I can also attach the .asc file if necessary.

Welcome.

> Why are there two outputs feeding the following stage?

Pin 15 connects to Ts6 Ts7, a very strong output. So pin 15 is the feedback input.

> It is not a classic Baxandall network, is it?

It is. (And not a passive James.) So you must have a Gain Stage inside the loop to get the intended response.

Rather than fool with 7 transistors, you can use a generic GAIN block. Ts1-3 is gain of +1, but if you drive directly with a SPICE infinite source, you don't need it. Ts4-7 looks like gain of about -680, and anything much over -50 will give near-right curves. (A lot of Bax were built around 12AX7 gain of -50.)

Thanks for your reply! I'll try that later!

I guess I got a lot to learn. Do you know any good literature on this topic?

So, I tried what you suggested and it works perfectly for the bass control, however the treble control doen't seem to do much.

Then I played around with the values and read this original article on the Baxandall network:

http://www.learnabout-electronics.org/Downloads/NegativeFeedbackTone.pdf

I noticed, that in the article (Page 4, Fig. 6) the central tapping of the potentiometer for treble control (P2) is shorted to the ground (am I interpreting the schematics right?), whereas in the schematics of the W295b there is a capacitor (C33, 150µ) in this wire.

In my simulation the treble control works better with smaller capacitor values (almost no change in frequency response with 150µ), highest boost/cut occurs when the capacitor is omitted. This doesn't seem to match with the short in the article.
Can anyone explain to me whats happening here?
Am I still doing something wrong?

Phillip

Your schematic pot representation confuses me. The 150uFd is supposed to the the grounded CENTER-tap. (Grounded for AC, blocks DC.) The wiper moves the 0.01uFd cap left or right, but not the 150uFd. I don't think you can easily simulate that with the sim-parts you are using.

The bass pot center tap reduces errors from lop-sided pot tracks. Your simulated pot has NO tracking error. Therefore you do not need the center-tap. And it has been shown (most commercial products) that omitting the center-tap works OK even with real/commodity pots.

Yeah you were right again. It's working with multiple resistors now, just not really handy. I found a post from Etheory were he showed some of the switches he programmed for this purpose. I think I'll try to use these.

However I am not done with the circuit...

In the mid boost/cut section I see this LCR network in some kind of feedback from this last amplification stage. My simulation works well for the cut, but doesn't work for boost.

I then simplified the LCR network to understand it better which led me to the attached circuit.

If the switch is turned to either boost or cut the resistors R75 and R76 are in series and the LCR is either before or after the resistors R75/76.

The circuit I simulated is cutting at the desired frequency if R1 > 0, but doesn't do anything if R1=0.

Is this a problem of the simulation or is something wrong with my circuit?

How does this feedback loop work anyway? I guess for boosting mode the desired frequencies are cut out of the feedback which leads to more amplification of those frequencies and for cutting its the other way around. Am I right about that?

milchmannverleih said:

It's working with multiple resistors now, just not really handy.

Click to expand...

You need to search the files in the LTspice group; there is a part named potentiometer_tapped, that does exactly what you want. You need to include the .sub in your .asc and write a .step directive that will sweep the potentiometer range.

milchmannverleih said:

I then simplified the LCR network to understand it better which led me to the attached circuit.

The circuit I simulated is cutting at the desired frequency if R1 > 0, but doesn't do anything if R1=0.

Click to expand...

That's correct.

Is this a problem of the simulation or is something wrong with my circuit?

Click to expand...

Over-simplification!

How does this feedback loop work anyway? I guess for boosting mode the desired frequencies are cut out of the feedback which leads to more amplification of those frequencies and for cutting its the other way around. Am I right about that?

Click to expand...

That's right. You need to include the RLC circuit and the gain block with both its inverting and non-inverting inputs to visualize boost and cut.

> doesn't do anything if R1=0.

"Zero" in SPICE means dead-zero. And a SPICE Voltage Source is a dead-zero impedance. You could bolt a 4-inch simulated Silver strap across it, flow 10,000,000 simulated Amperes, and it would *still* be 1 Volt.

abbey road d enfer said:

  That's right. You need to include the RLC circuit and the gain block with both its inverting and non-inverting inputs to visualize boost and cut.

Click to expand...

In which way do I have to connect the +/- and the LCR Feedback?

PRR said:

> doesn't do anything if R1=0.

"Zero" in SPICE means dead-zero. And a SPICE Voltage Source is a dead-zero impedance. You could bolt a 4-inch simulated Silver strap across it, flow 10,000,000 simulated Amperes, and it would *still* be 1 Volt.

Click to expand...

I get that, but shouldn't this give same result as replacing the 0 Ohm resistor with a wire?

I guess the problem lays in my simulation of the following amplification stage, but I'll ponder over it.

milchmannverleih said:

In which way do I have to connect the +/- and the LCR Feedback?

Click to expand...

Something like that?

Yeah well, thanks you guys!

It seems like you simply have to do everything correctly to make it work. 

One more thing..

If you would build this thing, which type of switches would you use? (shorting / non-shorting) Or does somebody know which was used in the original units?

Does it even make a difference in this/theses situation(s)?

To wake up an old thread...
How did it turn out for you eventually?
Did you manage to build it as intended?
If yes, would you care to share some of the documentaion of it?

Thank you for your time.
//Ted