THAT 1512 micpre noise issue

[timpanic]

Hi folks. I have a question and maybe somebody knows.

I built a micpre based on the usual schematic from the THAT documents. Simple 1512 with the usual diodes, caps in front with rf filter and a 1646 as output. Also pcb grinder etc used this design. Can also be found here a lot.

As rf filter I tried the 100pf and the 470/47p combi.

The issue is that when I combine more than 2 channels the channels began to produce noise/hiss at high gain settings. Especially when nothing is plugged in. When a mic is plugged in a noise is also there but it seems the channels interfere with each other at higher gain settings.

When I reduced the amount of chips installed in other channels and only use one or two channels the problem is gone so it seems they start to oscillate when more ics are plugged in but the voltage rails are all fine. Again each channel on its own works fine when no ics are installed. The 100n caps beside every ic are also installed.

BUT when I put a 100n wima cap over the + and - input lines, directly at the xlr connection or somewhere on the pcb before the 1512 chip the noise is gone completely.

So what is wrong here. I found a schematic for a single rail psu layout where such a cap was placed but with a lower value but this doesn't filter out all noise for me at the highest gain setting. I saw 8 preamps in 2he with this project with the same schematic so I wonder baldy what should be different there.

Til now every four channel preamp I built behave that way. Only when I build only two channels the issues does not appear.

Does anybody who has built any of the 1512 designs have an idea or any suggestions?

 

[Newmarket]

Wrt 100n blocking caps ? Do you mean bypass / decoupling caps ?
What is your summing circuit ?
Do you have a bulk decoupling caps where the power comes onto each board ?

 

[timpanic]

Thank you for your response. Yes I mean the decoupling caps. No summing. Each Pre goes to its own 1646 and seperate xlr out.
You mean caps higher than 100n near each ic ? I tried some caps on the powerrails beside the ones in the psu. Doesn´t make any difference. Also wonder why this isn´t there on any other designs. Here is the scheamtic identical with the design in the 1510/12 micpre documents from THAT.

 

[Bo Deadly]

Sounds like a grounding issue. How are you dressing the supply and ground wires to each board? Post a pic.

Is the GND of IN-2 and GND of C3 connected to pin 1 of the XLR in or to 0V shared by everything else?

 

[timpanic]

Sounds like a grounding issue. How are you dressing the supply and ground wires to each board? Post a pic.

Is the GND of IN-2 and GND of C3 connected to pin 1 of the XLR in or to 0V shared by everything else?

Yes the GND of IN-2 on this scheamtic is the same GND as the end of C3 and is shared with every 0V on the board. Is this wrong? Ground goes from the psu to the first board from there in series to every board with the +/- 15v ( like in a 500 lunchbox) and then from the last ( channel one ) to xlr pin1 input 1 and from there every xlr is grounded to the backpanel. PCB Grinder once had the same layout with a four pre. It had the same "issue" for me. Grounding there was also shared beside the 10R resistor which wasn´t the problem. As mentioned crossing hot and cold with a 100n filtered out a lot but still wondering.

 

[Newmarket]

You mean caps higher than 100n near each ic ? I tried some caps on the powerrails beside the ones in the psu. Doesn´t make any difference. Also wonder why this isn´t there on any other designs. Here is the scheamtic identical with the design in the 1510/12 micpre documents from THAT.

View attachment 102803

Thank you for your response. Yes I mean the decoupling caps. No summing. Each Pre goes to its own 1646 and seperate xlr out.
You mean caps higher than 100n near each ic ? I tried some caps on the powerrails beside the ones in the psu. Doesn´t make any difference. Also wonder why this isn´t there on any other designs. Here is the scheamtic identical with the design in the 1510/12 micpre documents from THAT.

View attachment 102803

So you're feeding the outputs into a mixer or interface to give the combined output ?
Not suggesting caps larger than 100n there. Talking about single pair of electrolytics where the voltage comes onto the board. Eg 2x220uF or whatever.

 

[timpanic]

So you're feeding the outputs into a mixer or interface to give the combined output ?
Not suggesting caps larger than 100n there. Talking about single pair of electrolytics where the voltage comes onto the board. Eg 2x220uF or whatever.

Yes, just how you would use a normal multi micpre where you need it, into a converter, interface, mixer whatever. The summing or anything after the micpre out does not have anything to do with the problem. I can hook up my signaltracer or the osci without anything connected to the unit and I will see a sudden hiss at the highergain setting which are not there with less ics installed or without the 100n crossing hot and cold. The problem clearly is related only to the 1512 and an oscillation going on at the input.


I just tried 220uf on the boards. No difference sadly.

 

[Bo Deadly]

Ground goes from the psu to the first board from there in series to every board

Unfortunately that will not work and that PCB cannot be salvaged. You must run supply lines to each circuit separately. This is because traces have inductance and resistance that, while very small, will cause small voltage potentials from currents. So any currents such as into / from 0V of the first circuit will be imparted onto the second circuit and then the third, fourth and so on.

Think if your 0V has like the "ground" that someone is standing on and each circuit is like a person. You want each person standing on the ground but, the way you have it, each person is standing on the sholders of the someone else and therefore the circuits become unstable.

 

[timpanic]

Unfortunately that will not work and that PCB cannot be salvaged. You must run supply lines to each circuit separately. This is because traces have inductance and resistance that, while very small, will cause small voltage potentials from currents. So any currents such as into / from 0V of the first circuit will be imparted onto the second circuit and then the third, fourth and so on.

Think if your 0V has like the "ground" that someone is standing on and each circuit is like a person. You want each person standing on the ground but, the way you have it, each person is standing on the sholders of the someone else and therefore the circuits become unstable.

HI. Thanks for the suggestion but then I wonder why every channelstrip console design and even a lunchbox design should work then.
In the last neotek console I recapped some weeks ago all channelstrips were combined with ide cables over meters. To say this will not work is a huge statement.
The pcb I posted was the 4pre from pcbgrinder several years ago. I wrote gustav about the problem but he says he didnt have any probs with the same design. can you explain that? So this design was allready wrong from the beginning?
I have a different pcb here with 2 channel pcbs. I just connected these. That would surprise me hard if the prob disappears when I change just the cables each direct to the psu.
Also I saw a dozen micpre designs where the modules are just connected with a big brandband cable in series. Then this was also all wrong then.

So you mean when I go with +/- 15v from every module directly to the psu pcb this should change the situation even if they are all on the same rail/cable/metall then again? EDIT: Checked..does not make any difference. Problem is still there.

Maybe you misunderstood me. They are in parallel connected in the circuit naturally but in series just from the physical position.

 

[ruffrecords]

HI. Thanks for the suggestion but then I wonder why every channelstrip console design and even a lunchbox design should work then.
In the last neotek console I recapped some weeks ago all channelstrips were combined with ide cables over meters. To say this will not work is a huge statement.

That is not quite what he said. Separate modules connected with ribbons cables are indeed common but are plagued with problems. It is better than your PCB latout but usually several wires in the ribbon cables are used to reduce inductance and the inductance of the wire in ribbon cables is much less than that of thin PCB traces.

The pcb I posted was the 4pre from pcbgrinder several years ago. I wrote gustav about the problem but he says he didnt have any probs with the same design. can you explain that? So this design was allready wrong from the beginning?

Designing this kind of PCB takes a lot of experience. I have to agree with Bo Deadly, this is not the best designed PCB I have seen.

I have a different pcb here with 2 channel pcbs. I just connected these. That would surprise me hard if the prob disappears when I change just the cables each direct to the psu.

Just to be clear, are you saying a different PCB with just two mic pres on it has the same problem?

Also I saw a dozen micpre designs where the modules are just connected with a big brandband cable in series. Then this was also all wrong then.

No. Big cables are different to small PCB tracks.

Cheers

Ian

 

[timpanic]

As I said several times now. It´s not my design but from pcbgrinder. Gustav, a nice fellow and quite a name in the scene here. There are a lot of boards like these out there.

Yes I just printed a pcb with two channels on a small pcb. Works like a charme with two channels alone but the prob starts when connecting more like in the pcbgrinder design and the ground or rail layout does not change anything and I tried a lot there. It´s more the 1512 receive some hiss from the inputs.

I also had this pcb grinder 4pre board and had this problem. Didnt solve the prob back then and just put the pcb back on the shelf

I then made my own 2 channel pcb and it works nice with two channels. Now I just discovered that when combined it produce the same problem.

The traces are not thin at all.

The prob is gone with the mod like crossing hot and cold with a cap I said but then I created another filter for sure.

 

[timpanic]

Here is the same circuit with 8 pres from here:
http://wiki.diyrecordingequipment.com/projects/pcb-grinder-pre-grinder-preamp/
Mine is wired the same.

 

[Bo Deadly]

The biggest problem with your board is the lack of a ground plane. Performance will depend a lot on routing, trace width and copper thickness. If a ground plane were used and rails were capacitively coupled to it locally, that greatly reduces 0V resistance and 0V noise. So it's really the 0V trace that is winding it's way up and down all over the place across the entire PCB that is likely at fault.

If you look at consoles, many times you'll see that the 0V is a "bus bar" running the length of the console. This is a thick strip of metal that makes the inductance and resistance really small.

You might be able to hack it to work. Just to prove that what I'm saying is in fact the problem, cut the 0V trace between the last two circuits and tack a 22-ish AWG wire directly to a 0V point in that circuit and then run it back directly to the 0V point on the power supply connector. Meaning bypass the ground trace with a fat wire.

Another thing you could do is find places to tack on 10uF electrolytic caps between the rails and 0V local to each circuit. That might help stablize it.

You could also use 100uF caps at the power entry connector.

But without a ground plane, I'm sorry, but this board is not good.

I don't know what "pcbgrinder" is but there are many instances where people have created and sold boards that people think are good designs and they're just not. Circuits like this tend to be stable until they're not so it might seem ok but with one little difference it all goes to pot.

 

[timpanic]

okay I will go on poking around then it seems.
I already tried to go directly from each modul to the power supply connector. With 15 +/- and with ground. i can try a bigger cable also.
pcbgrinder is the old project by Gustav who now runs goly.dk

What I now did was to reduce the gain under 60 db so when every channel is at lower gain settings the circuit is stable so far.

 

[FIX]

You can probably salvage this board (if you are only building this one) buy running some heavier gauge wire from the ground points at each amp to the main ground, then add some 100pf caps from the input lines to ground are pretty typical, as is a 470pf across the lines as it goes into the preamp, IN+, IN-. I would also increase your phantom power from 10R to 100R. R7 should be 0. Use this board to get it all working, then add the ground plane and the changes. Make sure that the preamp is the problem and not the output amp. they can be unstable as well. You can put 100pf to ground on the outputs as well, after a small ferrite bead.

 

[Matt Syson]

The issue is that when I combine more than 2 channels the channels began to produce noise/hiss at high gain settings. Especially when nothing is plugged in. When a mic is plugged in a noise is also there but it seems the channels interfere with each other at higher gain settings.

Well for a start you NEVER test mic preamps (particularly) without an input termination (a resistor of around 150 Ohms typically) AND your wiring to the input sockets must at least be twisted pairs and then again dressed to be well clear of any output wiring. THEN if your wiring has grounds bused to the XLRs like in the photo, that too is incorrect and should be pin1 to chassis at each XLR. THEN each amplifier section/board should have resistance and capacitance 'isolation' from all other channels (say 20 Ohms and 47uF or more.. The data sheets from chip manufacturers are the 'bare bones' of a circuit and it is up to you as a 'designer to add all the other parts that will make it into a design that is fot for the real world of radiated and conducted interference, voltage spikes etc. Outputs of op amps need 'isolation' resistances to prevent oscillation when confronted by a capacitive load (circuit traces/cables etc).

 

[ccaudle]

Yes the GND of IN-2 on this scheamtic is the same GND as the end of C3 and is shared with every 0V on the board. Is this wrong?

That is a well known mistake generally referred to as a "pin 1 problem" because all of the interference current from the cable shield can now go directly to your circuit 0V reference. The cable shield connection (pin 1) and the EMI filter caps should connect directly to the chassis at point of entry.

 

[Newmarket]

Just adding a note to back up the low impedance ground bus point. I used to be familiar with a "Big Desk" manufacturer where a copper bus bar of several sq mm was soldered to the PCB track to "beef up' the ground. I think the technical marketing blurb was along the lines "Military Style Multi-Point Grounding". Ie see what works best in a given installation
And yes IDC bussed desks are a bit notorious for developing problems. But this often due to the PVC insulation becoming brittle over time and the thin conductors (typ 28 AWG) fracturing.

 

[ruffrecords]

Quite often, spurious oscillations appear as noise/hiss to out ears. They are often casued by poor layout of poor screening between channels. They can easily be supersonic oscillations but they manifest themselves as noise. I would advise you to check the output with a wide band oscilloscope.

Cheers

Ian

 

[Cranehazard]

I agree with Matt you need to decouple the negative and positive POWER SUPPLIES of each preamp and maybe even each chip with the stated 20ohm 47uf filter, they may be talking to each other through the power supply. Some preamp manufacturers go as far as having seperate +15 -15 regulators for each preamp module they are all fed from a +24 -24 main set of regulators. This also gives you another 90db or so of power supply noise rejection. I have to disagree with everyone who thinks this is a grounding problem. I second that you can't listen to a mic preamp with no load it will always be the noisiest with no load and quietest with the input grounded. As said above, listening test it with 150ohm resistors on the inputs.