Jensen as017 preamp Adaptation

GroupDIY Audio Forum

Help Support GroupDIY Audio Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.

Icegoldnixon

Well-known member
Joined
Feb 3, 2015
Messages
79
Hello everyone!  ;D
I'm an amateur who has enjoyed looking at everyone's projects here. I've decided to try one of my own.
A few years ago I pulled some tamura transformers out of a Teac 3a mixer, and have decided to use them in a Jensen as017 mic preamp circuit. Their ratio is 1:5 or so, so I figured they'd be suitable. Anyway, this is my first time laying out a PCB this complicated, so I've attached a screenshot of the KiCad file. The schematic is the as017 circuit exactly, with (possibly unnecessary) decoupling caps added.
What I'm wondering is: do I need to update the zobel network for this substituted transformer? (Looking at the Teac schematic, it's not obvious what different values I would use.) Also, any general comments on my probably bad pcb layout is much appreciated. Thanks!
 

Attachments

  • tamuraa017.png
    tamuraa017.png
    74.6 KB · Views: 93
Icegoldnixon said:
Hello everyone!  ;D
I'm an amateur who has enjoyed looking at everyone's projects here. I've decided to try one of my own.
A few years ago I pulled some tamura transformers out of a Teac 3a mixer, and have decided to use them in a Jensen as017 mic preamp circuit. Their ratio is 1:5 or so, so I figured they'd be suitable. Anyway, this is my first time laying out a PCB this complicated, so I've attached a screenshot of the KiCad file. The schematic is the as017 circuit exactly, with (possibly unnecessary) decoupling caps added.
What I'm wondering is: do I need to update the zobel network for this substituted transformer? (Looking at the Teac schematic, it's not obvious what different values I would use.) Also, any general comments on my probably bad pcb layout is much appreciated. Thanks!
There's not much that can go wrong with such a simple circuit, however where do you connect the 0V of the supply rails?
The decoupling capacitors (1uF) are enormous; they should be ceramic, not film, 100nF should be enough, but electrolytics should be added if the connection to the PSU involes long-ish wires.
The ground plane is not optimum; it probably doesn't matter much because it's a tiny PCB, but the ground should be laid out according to "ground follows signal".
The two (4?) decoupling caps should ideally meet very close to each other, and the "cold" leg of the output should join there, as the 0V.
Indeed, the Zobel network needs to be adjusted for the different characteristics of the input xfmr.
 
Ok. So I'm going to get super pedantic. Most folks here will roll there eyes at all of the unnecessary stuff I'm going to discuss but if I were on my 2nd post and looking for a critique I would want someone to walk through every thought no matter how trivial.

I would consider making separate ground planes. Each ground plane has a separate ground pad that can run back to the power supply and thereby eliminate possible effects of inductance and resistance in the wire.

SGND: The input is going to be amplified by potentially a whole lot. So any noise on the input ground is going to be amplified. For that reason it might be good to have a separate ground plane for what is referred to as "signal ground" on the schem. That might even be why they gave it a different name.  So SGND would be for all things "signal ground" right up to pins 2,3 of the op amp but dodge the power supply bypass caps.

DGND: Depending on the load of the output, that op amp may be pushing/pulling a lot of current to/from whatever ground the load is connected to which might leak into other stuff and get amplified causing noise. So everything from the op amp output and beyond could have it's own ground plane.

PGND: Everything else like the op amp and power supply bypass could have it's own ground.

Then add solder jumps so that you can bridge SGND to PGND and PGND to DGND. Bridging either of these jumps is probably not going to impact performance depending on how noisy your PS is and what the output of the board is connected to but what could actually cause a real noise issue is if DGND is connected to SGND. Meaning the noise of the output is making it's way all the way back into the input which is getting amplified. That positive feedback loop is probably the #1 thing I would pick on in your layout.

Similarly, as someone else pointed out, it is standard practice to make all ground returns follow their sources. So the power supply connection point for example needs to have it's ground point right next to the +-V supply because ultimately any current going in through +-V is going to need to return somehow. You want those supply wires to be close (gently twisted probably) so that the magnetic field created by a sudden change in current will be canceled by the corresponding return current in the opposite direction.

To tie the above concepts together, I would solder jump DGND with PGND and run the 3 PS wires close together and use a separate wire for SGND. That will de-couple DGND and SGND and give the input a nice quiet ground reference. To see the effect of this, look at the noise floor of the final product with a high quality "audio interface" and some spectrum analyzer software and then try it with a ~1k ohm source load and ~500 ohm output load to stress the noise floor of the circuit and with and without the separate SGND wire / solder jump to see if there is any difference in noise floor. Meaning amplify silence as much as possible and compare noise floors.

Your power supply coupling caps should be maybe a little larger capacitance like 10u because the op amp might be asked to handle a higher load than normal. But they can be cheap electrolytic (way smaller than the big film caps you have shown in your layout). And if you want to use a fast op amp like an LME49710 you need some ceramic caps like 0.1u (probably very small like your compensation cap footprint) because they are very low ESR and will stabilize the op amp.

Note that you cannot switch in an arbitrary op amp in this circuit because the noise performance is going to depend on the source impedance of the transformer secondary matching the input impedance of the op amp input. There is a note about this on Jensen's website on the mic transformer input page. Specifically, you have to check the input current / input voltage noise of the OA and compare that to the source Z of the transformer. I haven't checked LM49710 for this but being a bi-polar OA it's probably about right. But a FET input like OPA134 would probably be wrong. Having said all of this, the circuit is almost certainly optimized exactly for the NE5534 and using any other op amp would probably negatively impact noise performance even though it claims to have better specs (although adjusting the 35k7 load resistor with some trial and error might restore and possibly increase noise performance with a different OA).

You could make everything from the ferrite beads and beyond optional since you might want to use a separate output stage (although the "quasi-balanced" output is quite good as it does offer good ground loop noise rejection.

Note that you don't have to use those through hole ferrite beads. Maybe those were common back in 1995 but these days, the surface mount equivalents are very common and cheap.

A decent 10k rev log conductive plastic part is the super cheap Alpha RD901 which can be found from numerous sources like small-bear electronics, thonk maybe and Tayda. They have a lot of useless track at the ends but otherwise, I use these pots a lot and they're great (very low power but fine for small signal audio).

Now to be really pedantic, I would consider minimizing the transformer -> 1k -> pin3 op amp path because that is a very low level signal and after the 1k it is relatively high impedance. The trace probably isn't long enough to pickup RF but I would put that 1k right up agains the op amp pin 3. And similarly, the 10k0 and 100 should be right up against pin 2. Also it IS important that you use shielded wire between the XLR in and the transformer in. You need 2 conductor with a full shield around it. I don't know if braided vs foil matters (foil can make a noise when moved but you don't care about that).

Note that you don't need resistors that are 35.7k or 49.9R and so on. Those are just the theoretical values that the designer (presimably Jim Williams) computed with his slide rule. You can use 33k and 47R and so on. It won't make any difference.

And maybe add some mounting holes.
 
Wow! Thank you, pedantic is what I crave. Attached is a new layout image. I've left the pseudo-balanced output for now, seeing as I ordered the parts for two boards already.  ::)
I changed the decoupling cap footprints for different parts. I foolishly assumed that film caps were always better, but my board can be much smaller now. Mounting holes also added.
I've got a stash of 10k alps pots I pulled from the same board as the transformers, so hopefully they'll do fine. On the schematic, they have the chassis ground on the output. Should my earth/chassis be connected to DGND? Happy Memorial Day!
 

Attachments

  • tamuralayout2.png
    tamuralayout2.png
    238.6 KB · Views: 55
Icegoldnixon said:
I changed the decoupling cap footprints for different parts. I foolishly assumed that film caps were always better, but my board can be much smaller now. Mounting holes also added.
Youi need a solid ground between C4 and C7; your ground pour is wimpy wher it passes below L1.
You should jumper L2 just like you've done for L1. Your ground pour on the right is not connected to XLR pin 1; it should be.
The pot should be connected to the same ground as the secondary of the input xfmr.
Actually, you don't need three grounds; two is enough. Connect together the 1st and 2nd pours.
Now I would make the fixing holes 3mm, but it's just me...
 
Looks good.

You can put the ground plane on both sides. It probably won't help with performance but if you only put the ground plane on one side, the board tends to come out slightly warped. The only problem is it usually gets in the way of things visually so it's something to do at the last possible moment. It takes energy and chemicals to dissolve the copper so you might as well just keep it.

You might want to flip the polarity of your output capacitors. With the NPN input of the NE5534 I think the output offset will tend to be positive because the NPN needs to draw a little current to "bias" so that current across 35.7k+1k is going to make a small voltage drop which is going to be reflected on the output as slightly positive. Electrolytics have no problem with a few volts of reverse polarity so 10 millivolts isn't going to do spit but if you know it's going to tend to be positive you might as well orient them the right way.

Note that the 10k pot should be reverse log because as you turn CW the smaller resistance causes larger changes in gain. So you want logarithmic but it has to be reverse so that when it's full CW it's using finer adjustment. This is another reason why stepped controls are preferred because you can independently set the gain of each step to be uniform.

Make sure your mounting holes do not conduct to the bolt or you could potentially connect your ground planes to the chassis which would defeat the purpose of having separate ground planes in the first place.

This has nothing to do with your immediate board but note that the XLR input pin 1 should be connected to the chassis right at the input. If you used even a short length of wire to connect pin 1 to the chassis, RF could be emitted into the enclosure (the length of the wire determines the frequency of RF emitted so shorter means only higher frequencies get in / lower frequencies blocked) and possibly amplified by your circuit, or more likely, the RF could bleed out of another IO connection and into another piece of gear (which is to suggest that all IO connections should have proper RF filtering). For this reason, I like to use the XLRs that have pin 1 connected to a little metal spike in the screw hole so that when you tighten that screw it stabs the front panel. Of course then you need to make sure your front panel has continuity all the way to the earth connection that connects to the power supply.

Similarly, usually the XLR input should have ferrite beads / 100p caps to block / shut RF. But again these should be as physically close to the XLR as possible. I actually have a little board not much bigger than the vertical mount XLR on it that has SMD chokes (Wurth 74279215) and footprints for 100R / 100u RC phantom power filter (eventually you will want to use a large diaphragm condenser microphone which requires 48V power).

This leads me to what I think is probably the most important thing about any DIY electronics project which is grounding. The name of the game is grounding, grounding, grounding. There are lots of discussion here about grounding that you can search about but for now let's just say that even if your ground wiring follows your schematic, that doesn't mean it's grounded properly. Just like I mentioned before about the separate ground wire for SGND, it matters where the various ground connections converge (preferably next to the ground lead of the last filter cap of the PS) and that you don't have loops because EMI will induce currents in a loop of wire.

Again, I suppose most of this really has little to do with your immediate board but it should be considered as the various connections and grounding and RF filtering have to be solid or all of your delicate PCB layout is not going to matter.
 
abbey road d enfer said:
Youi need a solid ground between C4 and C7; your ground pour is wimpy wher it passes below L1.
You should jumper L2 just like you've done for L1. Your ground pour on the right is not connected to XLR pin 1; it should be.
The pot should be connected to the same ground as the secondary of the input xfmr.
Actually, you don't need three grounds; two is enough. Connect together the 1st and 2nd pours.
Now I would make the fixing holes 3mm, but it's just me...
Clearly we are sending contradictory signals here so I just thought I should point them out. I suggested connected pin1 to the chassis and not the PCB for reasons explained in my last post. And I recommended connecting 2nd and 3rd pours so that SGND has it's own "quiet" connection since that is going the amplified reference. Otherwise, yes the ground pour under L1 gets very narrow. Presumably this ground plane is on the bottom? Maybe just run it on the top too.
 
squarewave said:
Clearly we are sending contradictory signals here so I just thought I should point them out. I suggested connected pin1 to the chassis and not the PCB for reasons explained in my last post.
Not really contradictory. Rather complimentary. The ground pour around the xlr, output caps and ferrites may not need to exist. But if it exists, it should be grounded. It coulod be grounded anywhere because it's an electrostatic shield; no significant current goes through. However chassis ground is the best candidate. Indeed Pin 1 of XLR should be connected to chassis with a solid connection.

And I recommended connecting 2nd and 3rd pours so that SGND has it's own "quiet" connection since that is going the amplified reference.
We may differ here. The 1st and 2nd pour need to be connected, otherwise, the circuit won't work. The 3rd should preferrably be connected to chassis, provided L2 goes to the 2nd pour.
I don't really understand the meaning of "SGND has it's own "quiet" connection ". Unless the PSU is dirty, all the connections here are "quiet".
There are two main points regarding the actual real-world noise performance of this circuit:
  • the "cold" side of the input xfmr secondary should be connected to the reference point of the 5534 stage. That point is where C2 is grounded.
  • XLR pin 3 should also be connected to the 5534 stage reference. For a different reason (avoiding unwanted circulating currents), it should also connected as close as possible to the point where the decoupling caps meet.
 
squarewave said:
You might want to flip the polarity of your output capacitors. With the NPN input of the NE5534 I think the output offset will tend to be positive because the NPN needs to draw a little current to "bias" so that current across 35.7k+1k is going to make a small voltage drop which is going to be reflected on the output as slightly positive. Electrolytics have no problem with a few volts of reverse polarity so 10 millivolts isn't going to do spit but if you know it's going to tend to be positive you might as well orient them the right way.

The output caps are actually bipolar, but the footprint doesn't represent that. Is there still a difference? I'm reading through the other comments now, grounding is complicated haha
 
abbey road d enfer said:
We may differ here. The 1st and 2nd pour need to be connected, otherwise, the circuit won't work.
I wasn't suggesting that any ground planes not be connected at all. I was suggesting using a separate ground wire for the first plane back to the PS so that noise from currents on the others (such as from the op amp output) are not amplified by the input.
 
abbey road d enfer said:
You should jumper L2 just like you've done for L1.
...
The pot should be connected to the same ground as the secondary of the input xfmr.

I'm not sure what you mean about L1 and L2. How is L1 jumpered exactly? It just looks like its in the correct part of the circuit to me. Same with the pot being connected to the input transformer secondary ground. Are they not in the same ground already? Thanks!
 
Another layout with minor updates. I'm not sure where things have settled on the output XLR pin 1, but I've connected it to the DGND plane here. Would leaving the planes 2 and 3 separate until jumpering them together be too much of a compromise? That is, is jumpering them at the connector pads worse than connecting them as a unified plane? Thanks!
 

Attachments

  • tamuralayout3.png
    tamuralayout3.png
    248.2 KB · Views: 25
squarewave said:
I wasn't suggesting that any ground planes not be connected at all. I was suggesting using a separate ground wire for the first plane back to the PS so that noise from currents on the others (such as from the op amp output) are not amplified by the input.
Really? You would have one wire coming from the PSU's 0V to the input board, and another also from the PSU to the second board. Think of them as resistors. Any voltage developed in the second wire, due to current flowing will create a differential voltage between the 1st board and the second. This differential voltage should be cancelled if the gain pot is referenced to the same ground as the secondary of the input xfmr, however why create this differential voltage, when it is more logical and simple to have a single ground wire?
 
Icegoldnixon said:
I'm not sure what you mean about L1 and L2. How is L1 jumpered exactly?
L1 "jumps" from one area of the PCB to another; should be the same for L2.

  It just looks like its in the correct part of the circuit to me. 
No. On your board, L1 is referenced to the 2nd ground, when L2 is referenced to the 3rd one.

  Same with the pot being connected to the input transformer secondary ground. Are they not in the same ground already? Yes they are. I was just emphasizing it is important to do so.
L1 "jumps" from one ground pour to another; should be the same for L2.
 
Does L1 not need to be connected to the same ground as the 22.1k output resistors? I could connect the bead to PGND instead, but my power flags have it connected to DGND as the ratsnest shows in the attached image.
 

Attachments

  • tamurabeadjump.png
    tamurabeadjump.png
    184.2 KB · Views: 23
Icegoldnixon said:
Does L1 not need to be connected to the same ground as the 22.1k output resistors?
No, it's not necessary at all.

I could connect the bead to PGND instead,
That's what you should do.

but my power flags have it connected to DGND as the ratsnest shows in the attached image.
Your ratsnet should do what you want it to do; you must amend your schematic. Both legs of the output should be referenced to the same ground.
 
Icegoldnixon said:
Does L1 not need to be connected to the same ground as the 22.1k output resistors? I could connect the bead to PGND instead, but my power flags have it connected to DGND as the ratsnest shows in the attached image.
I would do it the way you had it. I'm not sure what abbey means by L1 being referenced to PGND. If anything the ground reference of the output is the input which is referenced to SGND. If you make L2 ground PGND there's not point in having a separate ground plane for the output. And as stated previously, having a separate ground for the output is really just being pedantic. The rationale for separating PGND and DGND is if the output was really dumping a lot of current into DGND. But that op amp isn't going to put out more than 20mA or so which isn't enough to make a difference. If this were a 20W power amp driving a heavy load like a speaker, it might be important to make the load return separate. But not in this application. So you could just make PGND and DGND the same which is what abbey is advocating.
 
abbey road d enfer said:
Really? You would have one wire coming from the PSU's 0V to the input board, and another also from the PSU to the second board. Think of them as resistors. Any voltage developed in the second wire, due to current flowing will create a differential voltage between the 1st board and the second. This differential voltage should be cancelled if the gain pot is referenced to the same ground as the secondary of the input xfmr, however why create this differential voltage, when it is more logical and simple to have a single ground wire?
Yes. Note that the only thing connected to the second ground plane are the op amp bypass caps. So yes there will be a differential between grounds which is precisely why the input ground should be separate because you don't want that differential bleeding into the input. I think you just said as much a few posts back no? You don't want the output coupled to the input right? So if Icegoldnixon jumpers the 2nd and 3rd ground planes this is precisely what he will have.

UPDATE:

Here is the schematic BTW just so that we're clear about the circuit:

Screenshot%2Bfrom%2B2018-05-28%2B18-57-21.png


The parts that correspond to the 3 ground planes (in order which you have been referring to as 1st, 2nd and 3rd) in Icegold's layout are:

SGND: "Signal ground" is everything connected to "SIGNAL GROUND" in the schem including the gain control cap.

PGND: "Power ground" is just the op amp supply bypass caps (2 10u electrolytics and 2 ceramics) which are not show in the schem

DGND: "Dirty ground" is for the load return which is the grounded end of L2 and the bleeder resistors. Again, making PGND and DGND separate was based on my "pedantic" instructions and would work equally well as the same ground plane.
 
squarewave said:
Yes. Note that the only thing connected to the second ground plane are the op amp bypass caps. So yes there will be a differential between grounds which is precisely why the input ground should be separate because you don't want that differential bleeding into the input. I think you just said as much a few posts back no? You don't want the output coupled to the input right? So if Icegoldnixon jumpers the 2nd and 3rd ground planes this is precisely what he will have.

UPDATE:


SGND: "Signal ground" is everything connected to "SIGNAL GROUND" in the schem including the gain control cap.

PGND: "Power ground" is just the op amp supply bypass caps (2 10u electrolytics and 2 ceramics) which are not show in the schem

DGND: "Dirty ground" is for the load return which is the grounded end of L2 and the bleeder resistors. Again, making PGND and DGND separate was based on my "pedantic" instructions and would work equally well as the same ground plane.
I've been away for some time, now I can elaborate.
The concept of dirty or clean ground is misleading.
A node is dirty only in relation to another node. So which one is the dirty one?
As long as everything is related to the same node, it is by definition clean.
Now, if ground is considered as a physical entity, such as a chassis or a ground plane, one area can be "dirty" in reference to another. It's a matter of good sense to make sure the nodes that must be grounded to the same reference are indeed.
Back to the case at hand, I don't see why these copper pours could not be joined, as long as the rail currents are returned to a single point, and referencing all other nodes to this central point, since the layout is done in accordance with "ground follows signal path".
 
abbey road d enfer said:
Back to the case at hand, I don't see why these copper pours could not be joined, as long as the rail currents are returned to a single point, and referencing all other nodes to this central point, since the layout is done in accordance with "ground follows signal path".
I think we're starting to mix up grounding issue principles (which is easy to do). My understanding is, and correct me if I'm wrong, that the "ground follows signal" rule has to do with EMI and magnetic coupling of noise into other parts of the circuit. Then you have parasitic resistance / inductance which is a separate issue and yes, I believe I'm in agreement that if all grounds are the same (and thus share the same parasitics), everything will all balance out and there will be no negative effects.

However, I think there's a 3rd issue (although it does have to do with parasitics) which is that, because the circuit in question is high gain, any noise on the input is going to be amplified and, if the output ground is connected to the input ground, that amplified noise will be fed back around into the input and amplified again and again less so each time but enough that the end result will be a higher noise floor.
 

Latest posts

Back
Top