Need help with a TLM 102 sized PCB for DIY LDC mic

[edenooo]

Hello all!! This is my first post here, so apologies if any of this seems strange or out of place here, this just seems like the best place to ask this question.

I've been working on making my own DIY LDC microphone as of late, I've found some success and have finished my first proof of concept with a cheap aliexpress PCB, a JLI TSC-1 capsule, a TLM-102 styled body, and some 3D printed eTPU internals for shock resistance, and to my surprise the mic works! But as I suspected the cheap aliexpress mic circuit has some pretty horrible self noise, not too much distortion from what I can perceive- but it's not exactly easy to tell when there's an excessive hiss at all times, but this was all expected, I just wanted to start with something cheap that wouldn't be a big deal to mess up

So... This is will certainly be the hardest part of this project, I need to figure out some circuitboard that will fit inside of a TLM 102 sized body, I have very few character preferences and just want it to be low enough noise and with little distortion, an absolute dream would be to somehow fit an OPA Alice type circuit inside it (Maybe with a triple layer round PCB?), but I know that's borderline impossible, realistically anything fairly low noise will satisfy me as long as it actually fits.

What does everyone recommend? I know this is probably way too complicated of a project for my first* DIY Mic build, but I tend to prefer diving head first into these kinds of things anyway.

 

[Khron]

But as I suspected the cheap aliexpress mic circuit has some pretty horrible self noise,

Well, you could try desoldering the JFET, bending the gate pin so it connects to the capsule wire in the air (away from the PCB), and reinstall it - "easiest thing first"...

 

[rogs]

The OPIC project uses the same op-amp family as the 'OPA Alice' project, but is simpler - and actually slightly quieter!

The simplest of all the OPIC options is the OPIC42 version It has a minimal component count, and uses phantom power instead of a separate voltage multiplier for capsule polarisation, thus saving even more components.
Using this option will reduce the sensitivity of the mic by around 3dB, compared to mic using 60v of DC polarisation, but with a noise figure of only around 8dB(A) that shouldn't be a problem.
The project notes suggest a stripboard layout, which is not really suitable for your circular TLM 102 requirement, but it is a simple circuit so it should not present too many challenges when making a PCB layout.

Just a suggestion...

 

[edenooo]

The OPIC project uses the same op-amp family as the 'OPA Alice' project, but is simpler - and actually slightly quieter!

The simplest of all the OPIC options is the OPIC42 version It has a minimal component count, and uses phantom power instead of a separate voltage multiplier for capsule polarisation, thus saving even more components.
Using this option will reduce the sensitivity of the mic by around 3dB, compared to mic using 60v of DC polarisation, but with a noise figure of only around 8dB(A) that shouldn't be a problem.
The project notes suggest a stripboard layout, which is not really suitable for your circular TLM 102 requirement, but it is a simple circuit so it should not present too many challenges when making a PCB layout.

Just a suggestion...

This may be a decent option, I have very good preamps so I'm not too worried about needing to drive the mic a little harder as a result of the lower sensitivity, especially with how low of a noise floor the OPIC42 has, thank you for the suggestion!!

 

[edenooo]

The OPIC project uses the same op-amp family as the 'OPA Alice' project, but is simpler - and actually slightly quieter!

The simplest of all the OPIC options is the OPIC42 version It has a minimal component count, and uses phantom power instead of a separate voltage multiplier for capsule polarisation, thus saving even more components.
Using this option will reduce the sensitivity of the mic by around 3dB, compared to mic using 60v of DC polarisation, but with a noise figure of only around 8dB(A) that shouldn't be a problem.
The project notes suggest a stripboard layout, which is not really suitable for your circular TLM 102 requirement, but it is a simple circuit so it should not present too many challenges when making a PCB layout.

Just a suggestion...

I made a PCB based off your OPIC42 suggestion, it follows the exact schematic with an OPA1461. Seems like it should fit inside the mic body perfectly!! But thought I'd ask someone who has more experience just do double check things before sending the order off to JLCPCB, so let me know if anything seems wrong or off, thanks!

 

[edenooo]

Well, you could try desoldering the JFET, bending the gate pin so it connects to the capsule wire in the air (away from the PCB), and reinstall it - "easiest thing first"...

I may very well try this in the meantime, it wouldn't hurt lol, worst that could happen is I break an $0.86 Circuit that's barely worth using

 

[Khron]

But thought I'd ask someone who has more experience just do double check things before sending the order off to JLCPCB, so let me know if anything seems wrong or off, thanks!

1) You wanna stay away from 90deg corners when it's not essential, especially under the passives in the lower-right corner of the chip

2) ... And even more especially when coming off pads of SMD components - the two i mentioned above, the top two electrolytics, etc

3) Are both terminals of the electrolytic directly left of the chip supposed to be connected together? I think not - they definitely look like they are, going by the red trace...
(Doesn't Kicad have any "design rule check"? You'll wanna run that and solve all the errors it spits out before even considering manufacture)

4) Visual symmetry's nice and all, but it doesn't always play nice with the most optimal trace routing

5) All that's on the bottom layer is 3(?) traces? That's pretty wasteful...

6) Are you having JLCPCB also populate / assemble the boards? Asking because the three resistors(?) "above" the chip look like 0402-sized, which you might not want to be handling manually, if at all possible (the phrase "sorting fly s**t from pepper" comes to mind)

---

 

[edenooo]

1) You wanna stay away from 90deg corners when it's not essential, especially under the passives in the lower-right corner of the chip

2) ... And even more especially when coming off pads of SMD components - the two i mentioned above, the top two electrolytics, etc

3) Are both terminals of the electrolytic directly left of the chip supposed to be connected together? I think not - they definitely look like they are, going by the red trace...
(Doesn't Kicad have any "design rule check"? You'll wanna run that and solve all the errors it spits out before even considering manufacture)

4) Visual symmetry's nice and all, but it doesn't always play nice with the most optimal trace routing

5) All that's on the bottom layer is 3(?) traces? That's pretty wasteful...

6) Are you having JLCPCB also populate / assemble the boards? Asking because the three resistors(?) "above" the chip look like 0402-sized, which you might not want to be handling manually, if at all possible (the phrase "sorting fly s**t from pepper" comes to mind)

---

Thank you very much, I'm not going to act like I know more than I do, so I'm going to take my time to make sure the design is proper, thank you so so much for your notes, it's immensely helpful

and yes, I'm having JLI assemble the boards, it would be borderline impossible for me to be soldering those 0402 sized resistors by hand lol

 

[Khron]

it would be borderline impossible for me to be soldering those 0402 sized resistors by hand lol

Not that you have to, there's plenty of space there for all 1206 parts even, which are much more... ehrm... "practical"(?)

And on a related note...

 

[edenooo]

3) Are both terminals of the electrolytic directly left of the chip supposed to be connected together? I think not - they definitely look like they are, going by the red trace...
(Doesn't Kicad have any "design rule check"? You'll wanna run that and solve all the errors it spits out before even considering manufacture)

I've ran the DRC and it doesnt spit any errors, but I also know sometimes software can say things are fine when they definitely aren't I'll see </3

 

[Khron]

I've ran the DRC and it doesnt spit any errors,

Ok, but with what rules? No idea what its defaults are.

https://forum.kicad.info/t/design-rules-for-jlcpcb/46087

 

[edenooo]

Ok, but with what rules? No idea what its defaults are.

https://forum.kicad.info/t/design-rules-for-jlcpcb/46087

I'm using EasyEDA, they have default rules that are compliant with JLCPCB if I recall correctly..? I very well may be wrong though

 

[Khron]

I'm using EasyEDA, they have default rules that are compliant with JLCPCB if I recall correctly..? I very well may be wrong though

If it doesn't complain about traces overlapping other traces that they shouldn't.... I dunno how much i'd trust that

I mean...

3) Are both terminals of the electrolytic directly left of the chip supposed to be connected together? I think not - they definitely look like they are, going by the red trace...

PS. On a side-note, not having component designators displayed on the top silkscreen (or at least in this board view) really doesn't help with "navigation", or relating it to the schematic...

Speaking of schematic - you seem to have the XLR2 and 3 shorted together, THREE TIMES... Careful where you connect C7, R5, C3 (pretty sure this is NOT supposed to go between opamp output and ground!!!)

 

[edenooo]

If it doesn't complain about traces overlapping other traces that they shouldn't.... I dunno how much i'd trust that

I mean...

View attachment 147338

yeah..... I realize how awful that is, i've addressed all of those issues, I'll continue iterating tomorrow (or today, rather) since it's late where I am, but thank you for your help and advice, I cannot thank you enough

 

[Khron]

yeah..... I realize how awful that is, i've addressed all of those issues,

"But wait - there's more!..." (see the added stuff at the end of my previous post)

AND!!!!! You have the opamp's output going into its NON-INVERTING input. That's how you make an oscillator.

 

[rogs]

I made a PCB based off your OPIC42 suggestion, it follows the exact schematic with an OPA1461. Seems like it should fit inside the mic body perfectly!! But thought I'd ask someone who has more experience just do double check things before sending the order off to JLCPCB, so let me know if anything seems wrong or off, thanks!

I've only just seen your post... there are a number of schematic errors... as Khron has already pointed out.

Remove the following connections:

• C7 to XLR 2
• R5 to XLR 1
• R5 & XLR 2
• R4 to XLR 1
• C3 to R2

Correct the folllowing op-amp connections:

• OPA1641 pins 2 & 6 should be connected. -- not pins 3 and 6
• C11 and R1 should be connected to OPA1641 pin 3-- not pin 2

 

[rogs]

Couple of further points ....

• C1, C2,C3 and C4 are all specified as 47uF 50v for simplicitiy, as space is not at a premium on the original project stripboard layout,
Although C3 needs to have 50v rating, C1 and C2 can be 47uF rated at 35v - and C4 as low as 47uF 25v - if there is any advantage from a space point of view?
(I'm afraid I'm not at all familar with SMT devices myself!)

• Are you sure R1 and R9 are avaialable as SMT devices? 1GOhm is a very high and unusual value... I've not seen tiny SMD versions of that value listed myself. But I'm a bit out of touch with SMT , so I could be wrong there?....

• You might notice that the photos at the top of the original OPIC42 project notes show R1 and R9 as conventional 1/4w resistors, mounted vertically so that one end of each is off the board..... I use THIS component.
C11 is connected between those 2 off board leads - as is one of the capsule terminals.
This is quite deliberate. That capsule termination point is VERY high impedance, and highly susceptible to contamination from flux and dirt.
That can create horrible noise problems. Keeping the R1-R9-C11 terminations 'off board' can help solve any possible problems of that nature...

 

[Khron]

1GOhm is a very high and unusual value... I've not seen tiny SMD versions of that value listed myself. But I'm a bit out of touch with SMT , so I could be wrong there?....

They are available, at least vrom Vishay; whether they're in stock or not is another issue...

 

[edenooo]

They are available, at least vrom Vishay; whether they're in stock or not is another issue...

• Are you sure R1 and R9 are avaialable as SMT devices? 1GOhm is a very high and unusual value... I've not seen tiny SMD versions of that value listed myself. But I'm a bit out of touch with SMT , so I could be wrong there?....

1GOhm SMT resistors are available, they're actually somewhat cheaper compared to the larger solder through ones when they're in stock, but there are very few 1GOhm resistors available in JLIPCBs inventory for assembly in general, it was either $2 SMT or $12 for much larger Solder Through ones (which is INSANE but I know it's just supply and demand)

As for why such highly rated resistors are used? Not really sure, I'm just following the OPIC42 schematic, but I'm hoping to learn.

 

[edenooo]

• OPA1641 pins 2 & 6 should be connected. -- not pins 3 and 6
• C11 and R1 should be connected to OPA1641 pin 3-- not pin 2

"But wait - there's more!..." (see the added stuff at the end of my previous post)

AND!!!!! You have the opamp's output going into its NON-INVERTING input. That's how you make an oscillator.

Wow I cannot believe I didn't catch this earlier, it was staring right at my face without me noticing it