Transformerless 51X card - THAT 1570? Green? Amek?

[bruce0]

I was wanting a cheap, lightweight (my racks are mobile) 51x preamp to fill out the empty part of my 51x racks for my mobile recording rig. 

I have been adding various flavors of preamps, but I don't want to just build a bunch of something.  I want to be able to wait, and take selective advantage of all the great ideas that seem to be rolling through GroupDIY.  I will continue to add clones and stuff that looks interesting to add to my bag-o-tricks, but right now, I want to get the empty channels populated with a high quality clean fast cheap build (yes, I said those in the same sentence).

I looked around for a transformerless design.  Bruno's 9k5's are good and i built 3, but they are one flavor, and not cheap, simple or fast to build.

I want:
No transformers - light weight.
Lots of headroom (so I can make mistakes and not pay for them in the field)
Super low noise - ideally fully balanced operation ( to be more forgiving in the field).
Cheap
Low parts count or at least fast to build.
I am thinking simple - Gain, Phantom, mic/line switch (perhaps as an option), phase (I thought I might lay out the card with option space, headers, maybe standoff holes, to add other capability (High Pass, Limiter, etc) so I could evolve future versions if I wanted.)
Oh yeah and I want to get at least 8 in the racks by summer.

Is there anything out there now that fits that bill?

I was thinking about a 51x green pre, or a 51x fully balanced Amek 9098 clone.  But then I started looking at the THAT 1570 chip.  Other than the one major drawback (no pins - qfn-16 smd only) it seems like a good fit. 

There are several example schematics for this chip.  THAT publishes a well spec'd out, which I could use and Rane has a simpler one (once you throw away the clip lights - I have meters.

I know there is a digital project getting rolling out there using the 5170 digital preamp control chip, but I don't need that.  The 1570 runs analog, and it will add expense and a whole bunch of stuff to learn (One reason I like analog gear is that it doesnt HAVE software!).

What I am wondering is, before I re-invent the wheel.

Is what I want out there now?  A board I can just stuff, solder and go?

What do you all think of the 1570?

Any thoughts on the design?  ( I have read all the 1570 data sheet, and the two AES presentations THAT made, and the DN140 THAT design note ( it has some almost complete preamp designs in it)).  I was thinking of modifying one of those, perhaps with a CMR choke, and maybe metering.

Related topic. Anybody have a good 1570 QFN-16 eagle footprint? I have been looking into the whole surface mount thing, and putting a QFN-16 eagle footprint together (there doesn't seem to be a good one in place).  That wants a thermal pads with 5 tented vias (not eagles favorite task) under a single pad to drag heat to the opposite side of the board.  And then the thermal pad is not at ground it is at V-, so you have to separate the bottom side heat sink from the ground plane.  Anybody want to share a footprint. 

I noticed in the digital thread a comment that said that the THAT demo board was 4 layer for better performance, but the design notes don't mention that, in fact they talk about managing parasitic capacitance a task where I would think a 4 layer board would add complexity.  Any truth to the four layer need, and what is that about?

Anyway...  I was thinking I could keep the parts count low, keep the layout small, I think I can surface mount that one chip with a cheap reflow station, and do the rest with through hole components.

Thoughts and suggestions please.

 

[volker]

Why not just go with the THAT1510/12 into a THAT1646? There is nothing wrong with the ancestors . Actually I have just designed a pcb for that, albeit for a rackmount job. They are already here, I can let you know in a few weeks or so when I find time to build. It would be no problem to mount these into a L-bracket, gain switch/P48/polarity/pad wired to the front and the appropriate connector on the back. Price per channel should be around 30€.

Concerning the QFN: I also designed a ready-to-go pcb for the 1570/5171 some time ago following THAT's recommendations. I just never followed up on that matter as it was done mainly for the fun of it, but time was needed elsewhere eventually. It's in Eagle, I can upload the library later. Also, you definitely don't need a four-layer board to make it work well.


Volker

 

[bruce0]

Volker:

Thank you sir!  The footprint would definitely be appreciated.  I have been trying to figure out if there is a way to meet the THAT specification of 5 small tented vias to a copper plane on the back of the PCB for heat dissipation without getting all sorts of overlap errors.  I have tried it 6 ways to sunday, but can't seem to swing it.

I think I have a layout that will work, but it requires that I "Approve" overlap errors. (maybe that is the way of the eagle world, but I would be interested in what you put together).

Re: 1512/1646 approach
I considered the 1512 That1646 approach.  But I was intrigued by the fully balanced signal path of the 1570. It would be simple, quick, high quality. But it would take me single ended internally in the preamp.

I had been into the green-pre schematic, and the supergreen (Amek 9098) schematic, and I thought I would try to make the signal path that was balanced all the way through, if possible. Sort of trying to do what Amek would have done if they had the chips back then.

And I also wanted to gain experience with the 1570 as a possible front end another project (more stuff to put in the 3 end slots of my GDIY racks (and my clone rack).


But I will take another look at the 1512/1646 approach.  (maybe I could set a card up to do either, with some sort of little daughter card.

And (sheepish grin) I wanted a reason to get a hot air rework station, which arrived today and is pretty cool for the super cheap price.

Please post or PM the footprint if you would.

 

[volker]

Hi,

I don't remember if I nicked the footprints from somewhere or if I did them myself. So be sure to check the connections of the pins and the dimensions before sending off the design.

If the errors bother you (yes, sometimes accepting them is the fastest way) there is an easy workaround. Delete the plane from the footprint and draw it in the board and place the vias. Now give them all the same name. The plane has to be a polygon and not a rectangle, otherwise it won't be a "signal". If you want the vias to be tented, set the limits parameter in the DRC->Masks so it is bigger than the drill used.


Volker

 

[bruce0]

I did read about that, but I couldn't figure out how to do it without deleting the WHOLE thermal plane from the part, and that is a precisely measured plane that helps align the QFN with the surface tension of the solder.... I think I am more comfortable approving errors than drawing that exact little 2.6mm square with a nicked corner.

Thanks so much for the part.  I will check it and of course I wont hold you responsible if i use it instead of mine and it does me in!


I will let you know how it goes.

bb

 

[bruce0]

You did save my tail... I had the footprint the wrong size ... Inexplicable...

I copied someone elses footprint and modified it.  The thermal plate and the pitch was wrong.



Anyway thanks.

bb

 

[volker]

Ok, good to know .

Re the tented vias, I didn't catch that in my last post, it was late at night and the brain slow. With a via you have the choice between leaving them open, which means they will be tinned (HAL, gold, whatever). Or you put the solder mask over it, which is called tented. The pad underneath the IC is left open/free of solder mask of course, so tented vias don't make sense there as well. And that reminds me that you need to put a rectangle a bit bigger than the size of the plane in the tstop layer, otherwise it will be covered by the solder mask. I didn't put it in the footprint itself, don't know what was my thinking back then...

 

[bruce0]

Thanks, I figured that out and I fixed that already.

I added soldermask, fixed the size of the thermal pad (was a little too big)  rounded the contacts to match the chip (these two things according to my research will help the chip self center) and put tents on the BACK.  I know the back tents seem odd, but the recommendation vias to heat sinks is to tent them on the back if you have to solder to them, this creates a sealed "can" which helps prevent the solder on the thermal from wicking out. 

I also added the tcream needed to make a stencil (even though I am not going to make one) and I put a ring shape of trestrict on the back side in the part so that when I flow copper on the back from the vias that copper is isolated (because the thermal pad on the 1570 is at -18Volts).  I will post the part back when I am done (I probably should test it first, this will be my first smd part done with a hot air rework station.

I still plan on dropping the vias on and the back side plane on the board rather than the part.


As far as the original post is concerned, I appreciate your help... other than you... all I hear is crickets.

 

[volker]

Thanks, I figured that out and I fixed that already.

I added soldermask, fixed the size of the thermal pad (was a little too big)  rounded the contacts to match the chip (these two things according to my research will help the chip self center) and put tents on the BACK.  I know the back tents seem odd, but the recommendation vias to heat sinks is to tent them on the back if you have to solder to them, this creates a sealed "can" which helps prevent the solder on the thermal from wicking out.

Rounded pads/plane are not necessary for reflowing in my experience, if they help I don't know. You might have noticed that I elongated the pads to the outside more than would be usual. The reason is to make it easier to handsolder the chip. That is also why I would leave the vias untented so you can solder the plane from the bottom side. I've never tried it through tented ones, so YMMV.

 

[bruce0]

i have "zip" experience in reflowing.... So thank you... I am happy for the advice.

I did notice the extended pads, and guessed the reason.  The tents I am just doing using specs (written up by Intersil) that I found onine, for QFN packages.  They recommended making the pad shape match the part pads to help with surface tension centering.  I didn't round the plane, but I did make it's size match the part thermal plane exactly.

Maybe I should leave the back untented as you say, but it is a copper pour heatsink, so soldering by hand from that side would be  pretty ... tedious ... or impossible.  I was thinking I was going to heat the board up (still figuring out how . maybe float it over a heat gun on rails?  Or get a helper to aim a heat gun at the bottom, or maybe just try to do it from the top before I place the amp ) and the just do it with hot air rework gun.  You sound like you have been around that block, does that sound like it might work?

I am totally new to this SMD stuff, having only done little repairs using an small tip iron and a solder sucker.

 

[volker]

If Intersil say so it probably won't hurt. I'm no expert myself, I just used the oven at my university a bunch of times. Paste was applied by hand without a stencil, but still way easier than any other method. There are several approaches you can take to tackle the QFN at home. Some videos will probably better explain than I can in too many words:

http://www.youtube.com/watch?v=c_Qt5CtUlqY
http://www.youtube.com/watch?v=d-f-SBC0GrU
http://www.youtube.com/watch?v=gnuqPFwQCdM


I've used a similar approach to the second video at home, worked very well. Therefore I did not only put in the vias, but also mirrored the plane on the bottom side, so the heat can be applied better. I used a flat angled tip that can be pressed really well to the pcb. Only I prefer paste for the plane instead of preapplying solder.

The hot air approach looks very doable too, I might give that a try some time. And since you have a regulated one I'm sure you won't have too much trouble getting a functioning process.