DIY RF Condenser Mics

[rogs]

The 'FET detector' may be a big step in the right direction!
Have to try this as well! (And maybe design a new PCB for it...)
I think you have almost reached the maximum performance from such a simple circuit.

Well the initial test results are encouraging! .......

At the moment, I'm using BM800 bodies for my prototypes, so there's quite a lot of  PCB 'trimming' required each time....
I've been testing out a configuration with a capsule mount that allows me to build a 34mm  capsule into an end address cardioid mic ... and the body and headbasket of the BM800 are ideal for that...

So, Ruud if you do consider a new PCB, a rectangular one of 65mm x 35mm  which will fit straight into 'standard' BM700/800  body would be a real help.
I realise it would probably mean some upright components, and wouldn't be as elegant as your first  design....... but it would save a lot of 'hacking'....
....Just a thought ! 

 

[Khron]

"Only" using 7.5mm pitch at least for diodes would free up some space. I use that pitch for 1/4W resistors too, on my boards - a smidge "tight" for some tastes, but saves some board space too

I realise it would probably mean some upright components, and wouldn't be as elegant as your first  design....... but it would save a lot of 'hacking'....
....Just a thought ! 

PS: If someone could confirm the outside dimensions and pin grid / pitch of those IF transformers, i'd be ready to whip up a quick board design ;D And i have my older boards to consult for holes to fit precisely BM800 bodies  :



[A couple hours later]

Found some apparently-similar-footprint inductors in one of the stock Eagle libraries, so... ;D

I went with a ground plane on both sides, as well as some via "shielding" of the signal going to the JFET, to hopefully minimize any pickup from the oscillator section. That may very well introduce some extra capacitances here and there, so there's a good chance some cap values in the front-end might end up needing tweaking.

 

[rogs]

Looking good ! 

Couple of  points .....
• I think you have the values of the 100n and the 1n caps at the top of the board reversed ?-- No big deal (the're the same size!)

• The Spectrum IF cans are supposed to be identical to the Toko 10K series  - so on a 7mm matrix
(see here: https://www.bec.co.uk/downloads/10K%20Series.pdf )...

The 1.5mm pin size shown for the locating lugs is a bit tight... those holes really need to be c.1.7 or even 1.8mm

• The 47uH inductors are more like 1/2W resistors in size. I think they would need to be fitted on the back of the PCB in the present configuration.

• Same with the 47uF 50V electrolytic... ideally it would be nice to have enough room to have the option of being able to use the 8x8mm  Multicomp MCMHR series ( http://www.farnell.com/datasheets/1520837.pdf )  if possible ?

Am I right in thinking that because it's an Eagle design, you have to buy the PCB from them... They don't give you the option to generate standard Gerber files?......Or have I got that mixed up with someone else?

But as I say - looking good..... nice job! 

 

[Khron]

- That's just where the designation is on the silkscreen, just outside the caps' outline; i recreated the latest schematic.
I just figured i'd go with "functional" instead of "pretty", at least the first time around ;D

- I'll have to edit that package a bit then, no biggie. [Edit - turns out it's quite a bit bigger; the initial one was around 7x7mm-ish)
- Fair enough, i'll spread things out a bit in the output section.

You must be confusing it with some other package. Unless they went that route with later versions - i'm still on 6.3.0 It's got a Gerber export script, which i've used before to get boards done in China.

How's this, then?
https://www.dropbox.com/s/c3hx3a0w3odip2w/Screenshot%202019-05-03%2014.04.06.png?dl=0
[I tried attaching an updated version here, but it "failed security checks" - go figure  )

 

[rogs]

Looking even better! 

Couple of further points...

• The capacitor across the top 4k7 needs to be 1nF, and the one connected to the top BC560 base needs to be 100nF....  just an ident change, so no biggie...

• Because of the height and position of the coil cans, the PCB will need to be mounted below the frame.... I think that the 10nF caps  in their current location may hit the corner frame  mountings?... and maybe the coils at the other end?...

(There's a picture of my latest modified PCB from Ruud's prototype design which shows the problem here: www.jp137.com/lis/BM800modRUUDpcb.jpg )

Like you I can't seem to attach anything to posts at the moment because of 'security issues' ...???

• It would be nice if you could add an extra capacitor (2.5mm spacing)  across T1 secondary?
There's  a schematic showing the extra cap ( C3 - marked 'SOT') - here:  www.jp137.com/lis/RF.AMX8.jpg

Good news about the Gerber files.....  my mistake!

 

[Khron]

There's no ident change necessary, trust me

I shuffled the output components around a bit more, and the "top" edges of the cans (ie. towards the headbasket) are 3.8mm from the edge of the board.  Would they need to be even further away from the edge?

Is the server storage for attachments full, or something?

[Later edit] Reshuffled the oscillator section a bit too...
https://www.dropbox.com/s/l5neky8tw94i0rf/Screenshot%202019-05-03%2016.32.27.png?dl=0

 

[rogs]

There seems to be number of slightly different BM800 frames around.....

I've taken a photo of the worst one I can find (corner 'fill in' wise ) and there is a jpg of the internal dimensions of it here:

www.jp137.com/lis/BM800.frame.dimensions.jpg

 

[Khron]

Hmmm... With those two caps between the cans,  ~25mm's about as close as i can squeeze them together.

But how "tall" (left-to-right, in that frame photo) are those corner-fill-ins, on the top and bottom corners?

https://www.dropbox.com/s/k1ylsyqh6vhxn4c/BM800frame.png?dl=0


EDIT: Actually, nevermind - i scooted the two mounting holes a couple mm to the left (towards the cans), and shortened the other end of the board by 1-2mm.

So now, the centers of the mounting holes are a smidge under 25mm from the headbasket-side of the cans, so about 1mm to spare before those corner-pieces The other end might still be under question, though...

 

[rogs]

The dimensions you illustrated are c.5.5mm....

The one thing that I'm still not quite clear about.... The IF cans footprint is on a pretty 'standard' 7mm spacing...

What I'm not sure about is how big the holes are.

The  two mounting 'tags' on the cans  need around 1.7mm - or even 1.8mm if those will fit!
The pin hole sizes need to be 1mm ideally...
You might get away with 0.9mm for guaranteed new cans, but if you ever need to re-use a can, the holes need to be 1mm...

They look quite small on your schematic??

 

[Khron]

https://www.dropbox.com/s/1isek1kegec5x4k/Screenshot%202019-05-03%2017.55.40.png?dl=0

For the cans, i went with the dimensions in the Toko datasheet you linked on this page, but i can edit the footprint to make the holes bigger, sure

But now i gotta get my rear end to rehearsals, we've got a gig next friday to prepare for ;D

 

[rogs]

Looking good now! ....
Yes I think the TOKO hole dimensions are a bit too tight for the Spectrum Coils.....I had to drill out the tag mounting holes on Ruud's prototype PCB....
That's not too bad  with a single sided PCB -- not such a good idea for plated though holes on double sided board! 

And 1mm holes (with appropriate sized pads) for the pins will give bit of leeway for those coils that are 'less than perfect'....

 

[Khron]

Can pins 1.8mm drill, winding pins 1mm drill.

https://www.dropbox.com/s/4ruzx87w8799aly/Screenshot%202019-05-03%2020.22.57.png?dl=0

PS: The board outline is 63 x 37mm, and the screw holes are 28.5mm away from the left-side edge (can edge).

Also, i "fattened up" the footprint for the output series inductors (10mm pitch, plenty of space on the sides).

 

[rogs]

Looking better and better! 

I think the only query I have now  is the overlapping of the two negative terminal holes for the different sizes of electrolytic  -
It looks like the nearer hole would take out about 50% of the further hole pad!... maybe an optical illusion?
The 3.88mm (larger) spacing is the preferred option if one  of the holes does have to go....

I think it's maybe time to try it out .... 
   
Are you going to publish the Gerber files? .. .. I'd love to order a few from China ASAP..

 

[Khron]

Running Itead's DRC does indeed give an error on that overlap, but it's a "drill distance" error, and it looks like the two holes would overlap the tiniest bit. Keep in mind the holes are 0.8mm diameter.

https://www.dropbox.com/s/6ztknaex5971beb/Screenshot%202019-05-03%2023.22.47.png?dl=0

I wonder, does your PCB fab of choice have some sort of checking-service before placing the actual order to make sure it's feasible?
Or some way to mention that this one detail is "ignorable"?

And sure, exporting the Gerbers is only a few clicks away. Should the silkscreen only contain the component outlines and values, or..?

 

[rogs]

I was going to order some prototypes from JLCPCB ...they do check the Gerber files, but I'm not sure what happens if they encounter what they see as 'errors'..

Re: the ident ... the ideal option is to include  the outlines and component references as shown on the schematic ...'R2' -- 'C4' -- 'T2'.
That way it's simple to change the  values on the schematic -, if necessary - without making the PCB then show the wrong value.....

But if that involves a lot of work, I think probably the outlines only, with a component reference listing on a separate document..

I can add the schematic references onto the latest  layout png if that helps at all?...

 

[Khron]

When i drew the schematic (you have to do that first, in Eagle), i used the same designators as in the latest schematic, so that should all be fine I'll just have to "drag out" the designators so they don't overlap the outlines or pads.

https://www.dropbox.com/s/q7dp73lcvvpbbq4/Screenshot%202019-05-04%2000.04.40.png?dl=0

How's this, for a silkscreen then? (Ignore the little "+" things, those are just the "origins" of the designator items, they don't show up in the Gerbers)

https://www.dropbox.com/s/po13lzckqoqyvpq/Screenshot%202019-05-04%2000.13.51.png?dl=0

 

[rogs]

Superb !  Exactly what I had in mind ( see here:  www.jp137.com/lis/RF.AMX8%20ident.jpg      )

 

[Khron]

Great minds think alike, or... something-something ;D

So let's see then - top silkscreen, top soldermask, top layer, bottom layer, bottom soldermask, and drills.  That should suffice, since there's no bottom silkscreen, right?

 

[rogs]

Sounds good to me...

 

[Khron]

Looks good on JLC's Gerber viewer

https://www.dropbox.com/s/sc1y3m0l4uvwxs8/RFmic_gerber.zip?dl=0

I also added some "soldermask stop" areas on the top of the board, to help ensure as good a ground-contact with the chassis as possible. Not sure if or how much that does, but it definitely hasn't hurt my Schoeps + DC-DC BM800 builds.

Granted, if one was to "cheat", there's a script somewhere for panelizing (ie. copying multiples of one board within a footprint, and correcting the designators - in this case, one could get double the boards for the same price, since they fit within the 10x10cm "cheap limit"   )