Layout tips please...

[3nity]

here's a pcb layout for the INA217 but that i think could be used with THAT1510.

The layout is based only on the preamp as Phantom/pad/phase are on another board with switches and a phantom led that would go on rear of the front panel.

At one side of R3 theres nothing as i expect to wire one leg of my Rev Log there to pin 7 of IC1.

i'm a newbie so don;t expect the greatest layout

 

[12afael]

what I do to make a jumper is draw with the botom layer then change to the top, draw another line(the jumper (in red)) and then change the layer to bottom again and draw another line. you must set the pad size and drill size.

try to use wider line, more easy to etch :wink: .

Rafael

 

[3nity]

gracias, estaba pensando en eso: wider lines.

but why the jumper??

 

[12afael]

sorry I thought you had to connect the pad near r3 to the pot. I didn´t see the wires between pads on J3.

 

[Ptownkid]

you're definitely going to want to increase trace width, which becomes a pita as the drc will spit out errors like crazy. It takes some time and practice.

 

[Samuel Groner]

There seem to be a few issues with the schematic. Need a bigger version which one can read.

Samuel

 

[peterc]

I have a rule of thumb:

Only single sided PCB's so I can home etch them & test for accuracy. My traces are generally .8mm (30 mil), makes it easy to avoid problems with thin tracks. I usually have a few links, but thats OK.

Peter

 

[3nity]

big enough for you? :thumb:

Before taking into consideration any word let me know how can we do another layout from the same schematic in eagle?

cheers.

 

[Ptownkid]

I'm assuming you want to save that brd file and make another? You'll have to rename and save.

 

[12afael]

save the schematic with another name, I`m not shure but maybe you must delete the *newname*.brd

 

[3nity]

thanks 12fael that worked! gonna work on that later....

oh by the way .8mm (30mil) would be fine as traces?

 

[Ptownkid]

yeah, 30 is pretty big, i usually end up between 24-26 and they etch fine

 

[Handcrafted Tone]

I prefer traces around 50mil, and 40 mil of isolation between. MUCH easier to home etch.

 

[owel]

Is the diameter/size of your C1 and C2 correct? They look big to me.

Bigger traces.

Avoid unnecessary bends... is this an autoroute layout? If so, you may want to play with the parameters.

My preferred method is manual routing, and just use Eagle as my guide by "lighting up" the pads I need to connect.

IS there enough clearance between D1 and IC1? What if you use an IC socket?

Power supply decoupling caps should be nearest the opamp supply pins. Always use them. I don't see any around your chips. Datasheet schematics don't always show them... because it's assumed you will add them.

No ground fills/areas?

Take care around the input area of IC1 and Rgain. These are prone to noise pickup if not done right.

 

[3nity]

thanks owel.
definetely working in a newer layout...i did improve it with your tips.

What values do you sugest for decoupling caps? i'd say 220uf/35v.
How you work your routimg manually? and waht about ground areas?

thanks!

BTW: before i posted this i read a few threas you post it when you were begining in pcb layouts!

 

[owel]

I meant 0.1uf/50V decoupling caps.

BTW: before i posted this i read a few threas you post it when you were begining in pcb layouts!

Yea, it took several false starts for me to learn Eagle. Tried other software packages (both freeware and shareware), and I always seem to come back to Eagle.

Graduated from the free version to the paid version (with a couple of modules) so the incentive to learn it more is greater

 

[12afael]

I`ve used protel, but I love eagle , you have more options on protel but eagle is a lot more easy, at least for me.

 

[Samuel Groner]

As a general note: it looks to me as if the schematic you posted where not that you used to draw the PCB e.g. as I don't see any part identifiers for the capacitors. It is of utmost importance to start with a cleanly drawn schematic that shows all the details and which sub-groups exist in the circuit (e.g. the servo).

Regarding the schematic a few notes (some of that has been already mentioned):
* The protection diodes should be 1N4007GP and not a small-signal type.
* For good phantom power protection you need small resistors (4.7 ohm) between input capacitors and diodes.
* I don't see any RFI protection--I want a pair of 1 nFs to chassis at the input.
* A2 wants a 100 nF decoupling between the supplies.
* A1 needs a 47 ohm-or-so isolation resistor at the output or it will immediately go into oscillation when seeing any capacitive load. Add another resistor to ground for an impedance-balanced output.
* I suggest to use a resistor in front of the 47 uF 48 V filter cap to form a more effective filter. About 330 ohm is fine.
* Keep pin 1 (chassis) and supply ground (audio ground) separate. Chassis is only used to ground the RFI protection caps.

Regarding the layout (some of that has been already mentioned):
* The decoupling capacitors for the ICs should be as close as possible.
* Think balanced--the two input lines should be routed symmetrical and in close proximity for best CMRR and immunity to induced hum.
* I'd add a ground plane, at least around the border of the board.
* Make sure to minimise trace length and any stray capacity at the gain setting network (R6/R7).
* Personally I prefer dual layer boards. Even for such simple circuits there are much fewer compromises that need to be done.
* Regarding track width: I go for 20 mil for the signal traces and 50 mil for the supply lines. I never etch myself though.

Samuel

 

[Infernal_Death]

Sorry if it's already said but you should avoid 90 degree turn traces. I am not experienced in drawing layouts but i remember to read that you should avoid them. Maybe some of the more experienced here can tell you why.
On the few layouts i did i always use all the room where no signal traces are as ground planes. Doesn't hurt and you won't use as much etching fluid as you would when you have to etch everything away.

Flo

 

[3nity]

Schematic updated.
Thanks Sam for all the advices.

As you can see i forgot to put values on C1 and C2 those are 1nF.
I put R7 following your advice dut i don't know the value so.

i also put decouplig caps.

one thing i'm not really shure it;s IC2 OPA137 pin 3 goes to ground or chassis??

cheers.