Jung SR schemo/layout

[daArry]

Hey,

I'm new to these improved psu designs but would like to try some for +30/-10V operation. Current load shouldnt go over the rated 1.5A max of the LM317 so from the published ckts I assume I don't need to change anything except the feedback resistors around the opamp to set the output voltage...

Here's a schemo I've drawn up of an exsisting schem found on this forum somewhere (of the + supply):



I've layed out a single sided PCB too: (inspired from designs whilst searching this forum):



We good to roll?

Cheers,

[jan.didden]

Originally posted by daArry
Hey,

I'm new to these improved psu designs but would like to try some for +30/-10V operation. Current load shouldnt go over the rated 1.5A max of the LM317 so from the published ckts I assume I don't need to change anything except the feedback resistors around the opamp to set the output voltage...

Here's a schemo I've drawn up of an exsisting schem found on this forum somewhere (of the + supply):



I've layed out a single sided PCB too: (inspired from designs whilst searching this forum):



We good to roll?

Cheers,

Yeah, looks not bad.
Couple points (in the positive spirit): C2 is a waste. The diode will have a dynamic impedance of say 1 Ohm. Plus the intrinsic emitter resistance that is unbypassed. That 100uF will not measurable change things, let alone audible. It takes up too much PCB space.

The PCB can be improved.
At the left, the area C1, C9, C8 can be MUCH tighter, making for shorter connections. Rotate caps for shortest tracks. On the right side, R7, ZD1, RV2, R5 should be moved directly close to the opamp. C4 can be rotated, all to give a smaller, tighter PCB. Don't make wide tracks for small-signal lines. they take up too much space. Wide tracks here only make sense for the input, output and ground lines. The rest is all small-signal.
But your layout is clean and the grounding looks OK to me.

Jan Didden

[daArry]

Hi Jan,

Thanks for your comments - here's an updated layout:



Much smaller brd size now

All the best,

Dan

[carlmart]

Originally posted by daArry

Thanks for your comments - here's an updated layout:



Much smaller brd size now

The board looks great now.

You could accomodate things a bit more by moving Vout out to the border of the pcb and GNDout to be just below it. As it is now it's difficult to get to.

If you rotate C5 clockwise and move it up a bit you might be able to do that.

On the lower side C6 could be rotated to be 90 degrees to the IC, allowing a bit more space for different types.

Include AD817 as a DIP option to the AD797, which seems to be a "conflictive" option.

If you are considering an only-SOIC part as the AD825 you should put the tracks for it on the pcb, if you are designing it from zero.

One of the good things of the Jung regulator was the "sensing" ground. Aren't you implementing any?


Carlos

[daArry]

Hey Carlos,

The reason for the placement of the vin/vout, gnd_in/out holes was so I could sit the pcb on vero stripboard and each would have it's own copper line from the off. Then, on one end I'd have the rectifying ckt and the other the regulated outs on screwfix connectors...

Thanks for the heads-up on the opamps - for the smd only parts i was gonna attach the part to a dip ic socket by bending the legs outwards and soldering it underneath...

WRT the sensing ground - from what i've seen it's all joined up somewhere along the way anyway so I was just goin for a quicker solution by attaching all grounds on the brd from the get go...or have i missed something?

[carlmart]

Originally posted by daArry

WRT the sensing ground - from what i've seen it's all joined up somewhere along the way anyway so I was just goin for a quicker solution by attaching all grounds on the brd from the get go...or have i missed something?

Well, you missed why the grounds should be kept separate and only joined at the powering point, close to the device you are going to power.

Perhaps you should read the original Gary Galo article on the matter.

Whether this issue is important and how, it would be nice to hear from others too.

Carlos

[daArry]

Yer, I (try n') aim for a star/central point system when grounding so I guess might as well here then eh

Here's a tweaked layout with the 0Vsense pin:



Thanks again,

Dan

[peranders]

Looks good but here are a couple of thoughts from me:

C6 is probably to no use at all becasue of the long traces and if you put it nearer the output you would probably get oscillations. I solved this by inserting a small resistor between output and pin 7 of the opamp. By this achieving good decoupling of the opamp and isolate a bit towards the output.

You may move T3 a bit and there draw the trace from the out to the LM317. You need only a small trace like 20-30 mil. By this you will remove a rather long loop. It may not be important.

You can also make some small adjustments in order to get a more compact solution.

T1 up a bit
D1 up and left
T2 left
IC1 left

Out connection up, left

C3 left

and the rest of the package a bit left.

Strive to have a fatter ground trace.

Maybe 100 nF at the input would be appropiate.

I wonder also have much good D3, D4 along with modern opams.

15 V out than a real short circuit.

Pin 7 0 V
Pin 3 +7V
Pin 2 -7 V
Is this enough to damage an opamp?

With diodes:
Pin 7 0 V
Pin 3 around +-1 V
Pin 2 around +- 1 V

and not more than 0.7 volts between the inputs.

If you happen to have more gain than 2 or less then you will get several volts above or below pin 7 at the inputs.

So in real life under normal conditions, how much good do those diodes. They do no harm, I'm sure. Maybe add some capacitance but compared to 500 ohms impedance it's not so much.

[Greg Erskine]

hi daArry,

Looking good.

After a quick look the only point could make is the size of the pads on a single sided board "may" need to be larger. I find most standard components seem to be designed for double sided PCBs. Just a word of warning: I've never actually made a PCB.

[peranders]

Good point. 75 mils at least is OK.