need help in pcb board layout for LM7721

Hi Sami,

The circuit looks correct, but you need to connect the guard and guard pins. The 7721 "Guard" pins are not internally connected and there is no "driver" inside.

The guard should be connected to probe common potential (the shell of the BNC). Don't confuse the "grounds"...I would not call the probe shield "ground" as it is 500mV above ground.

The most critical part of the circuit is the path between the center terminal of the BNC and the input of the buffer amplifier (U2-Pin1). As you have done, the signal node from the BNC to the amplifier should be completely surrounded by the guard trace - on BOTH sides of the board (since the BNC is thru-hole).

On the bottom of the board, the plane immediately above and surrounding the connector input pin should be guard - not ground. In other words, the BNC connector should be "floating" on a guard plane isolated from ground.

The rest of the layout is DC and is not too critical. IC1 does not need to be a LMP7721 since it does not require low bias currents. it is just buffering the reference voltage. A LMP7715 can be used instead (same family).

Regards,

hi Paul !

please review the new circuit as i replaced IC1 by LMP7715.

>>The circuit looks correct, but you need to connect the guard and guard pins. The 7721 "Guard" pins are not internally connected and there is no "driver" inside.

I think its ok now please confirm.

>>The guard should be connected to probe common potential (the shell of the BNC). Don't confuse the "grounds"...I would not call the probe shield "ground" >>as it is 500mV above ground.

have i connected the guard correctly to the shell of BNC? I am assuming that the two larger size legs are the shell of BNC.

>>the signal node from the BNC to the amplifier should be completely surrounded by the guard trace - on BOTH sides of the board

if I do this then how do I trace the unrouted net line (as seen in the diagram with yellow color) to the BNC connector since the guard lines on both sides will be in the way?

>>On the bottom of the board, the plane immediately above and surrounding the connector input pin should be guard - not ground. In other words, the BNC >>connector should be "floating" on a guard plane isolated from ground.

I did not understand this ,please explain again.

Also should i connect the guard line to VCC and at any place ? and on both sides of the board ?

hi Paul !

I just noticed that the two large posts on the BNC are just for the mounting support and are not seen as "connectors" in the eagle cad software so it does not connt the guard to it , so which pin is the "shell of the BNC"  to which I should connect the guard to?

thanks

here is only the TOP layer so give you a clearer picture. as you see the guard trace is not connected to the large two posts of the BNC connector , iam not sure if thats the shield or not. Also if I put the same guard trace down on the bottom layer then it puts VIAs and connect it to the upper trace , but I dont think thats what is required, so how do i put the bottom guard and how should it be connected to the upper guard ?

and how do I route this unrouted net line from the resistor to the GND pin of the BNC since the guard line is in the way ? 

hi Paul !
few things i am confused about :
1- the guard is supposed to be connected to ground or VCC?
2- i found the demo board at <www.ti.com/lit/ug/snou004/snou004.pdf > but its different, it has kind of two Guards , and pin1 and 8 are both guarded.
3- P$1, P$2, P$GND of the BNC should all be connected to guard ? but then what you meant by earlier in the post that the shield of BNC should be kept seperate from GND? i am sure i didnt understand it properly.
4- what to do with the PS$GND pin?

please check the board above i have modified it to the best of my understanding, and i will use the metal BNC as per your advise.

pin8 of IC2 could not be routed so can i use a VIA and bring it under the board ? 

below is the top and bottom layer and bottom solder mask is  connected to the BNC mount posts (PS$1, PS$2) , did i get it right? 

thanks
Sami

Hi Sami,

Sorry for the delay, I was traveling.

1. Neither. It should be connected to 1.25V through R3 - same as the probe "shield" pin. R3, the shell of the BNC, and the "guard" plane should be connected together.

I would not label the shell of the BNC "GND" - it is confusing. It is not ground. It is the probe common that is 1.25V above ground, driven by R3 & IC1. Maybe call it "P$COM".

2. It only has one guard. The connector is a "triax" connector. It looks like a BNC, but it has a third "ring" inside that surrounds the center pin. Pins 1 & 8 are eventually connected together through the guard traces. There are identical guard rings on the top and bottom of the board - but they are all connected together.

3. Yes. P$1, P$2, P$GND and R3-2 should all be connected together. Pull the copper pour over the ground pin (see pic below).

4. Connect it to R3-2.

You do not really need to connect pin 7 as pin 8 is a "low impedance" node. Though it would be good to connect it to the guard plane. Move the copper pour over a bit to get some room to move things around. There looks to be a path around R4 to route pin 8 to R4-2.

Regards,

hi Paul !

I am very excited to work on this project with your help again. I did my best to try to follow your instructions but I am sure I didnt get it all of it right, so here is my layout and circuit , what did I do wrong?

few points of confusion :

1)you said "3. Yes. P$1, P$2, P$GND and R3-2 should all be connected together" , but isnt P$1 and P$2 the shell of BNC and connected to the guard ?and if this is the case then the guard also gets connected to GND  . if you look at the board layout you will see that P$1 ,P$2 are connected to the copper pour on the bottom layer which is GND, and on top layer I have connected P$1, P$2 to guard shown with red lines.  is this correct ?

2) I dont have any guard on the bottom , should i place one down also?

3) I introduced a via on pin6 of 7721 , will it cause issues ? its a VCC pin.

here is my design if you can mark/draw  the corrections please and thanks for being so patience with me.

Hi Sami,

DO NOT ground P$2, P$1, P$GND and R3! .

P$2, P$1, P$GND, R3 and IC2-6 form the "Sensor Common" line, which is also the guard. The copper pour should be connected the guard node and NOT ground.

Remove the ground triangle and it is wired correctly:

P$1 and P$2 will be the same as P$GND (BNC shell) with the all-metal body connector.

I would put an identical copper pour on the opposite side. The pours can be connected through the P$1 and P$2 mounting holes.

The via should not cause an issue.

Regards,

hi PAul !

iam a little confused , if the guard is copper filled then its all one area of copper whats the meaning of "guard" in that sense? 

here are the top and botom layers , please review

here is the circuit diagram . 

Hi Sami,

You are getting close. The circuit is correct, but now the "guard" copper pour (and P$1 and P$2) are not connected to R3.  Connect P$1 and P$2 to the P$GND and R3 node.

I would also increase the spacing around the P$SIG trace. It is a little closer than I like. Pull it back about a mm or two. I'm not too familiar with Eagle, but usually you can place a copper pour keep-out over the input pin to remove the fill copper in that area.

1. Connect the guard plane

2. Put some space around the input trace

Here.....make it look like this:

Regards,

hi Paul !

thanks for being patience with me and thanks for all your help, its a complex undertaking for me but yes we are getting closer.

1)

you wrote :

"The circuit is correct, but now the "guard" copper pour (and P$1 and P$2) are not connected to R3.  Connect P$1 and P$2b to the P$GND "

but they are connected since the top red layer which is the copper fill is connecting the P$1 and P$1 ( red crosshairs)  but its also connecting the

P$GND (red cross hairs) . 

please see the blow up picture below and advise .

2) connect the guard plane .  

where do i connect it ? its actually hidden under the copper fill  but its connected to the PS$1 and PS$2 and since PS$1 and PS$2 and PS$GND are all connected via

copper fill the guard plane is also connected to them .

below pic i hid the copper fill so its showing how the guard is layed out.  here you can see much better that PS$1, PS$2 andPS$G

are all connected via a wire and when i do a copper fill (as shown in above picture ) it also gets connected to the PS$1 and PS$2 .

i explicitly connected the P$1, P$2, P$GND and copper fill and guard , please review the top n bot layer.

Hi Sami,

The layout looks good now. I would pull the copper back a bit (more of a gap) around the "P$SIG" (center pin) on the bottom (blue) layer.  Maybe a 100 mils (~2.5mm) gap.

But looks like you have still grounded the guard through pad "2" in the lower middle and goes off to pin 3, which is GND.

Please run a LVS to make sure the connections match your schematic.

Regards,

good catch Paul , i have made all the corrections . I couldnt increase the gap to 2.5mm arouind the P$SIG as it merges with the P$GND then . the gap now is around 1mm is it ok ?
I have removed the connection between pad2 and pad3 it was mistake. 

Also i am not understanding this , if the guard and the copper fill are both connected to P$1 and P$2 then they sould be merged right?  please see the image below.

I have put this together to the best of my understanding please review.

since you are very busy is it possible to have a 5 mins phone session with you so we can hammer this out please?

hi Paul !
attaching the new pics, i bridged the gaps and cleared copper around the P$SIG to maximum .

obsolete

Hi Sami,

The schematic looks good. Just make sure the PCB connections match.

Regards,

below are the three  snapshots , of top both layers,  top layer,  and bottom layer respectively.

regards

in the previous post i posted the layers of the the ph meter below i am posting the ph meter actual layout on the controller board with

other componentss.  pics ,of in circuit layout showing the actual ground and FILL  , please see if this is ok .

first pic shows both layer n the second picture shows bottom layer.

as you see there is no connection between FILL and GND  ..i think thats what you wanted ?

hi Paul !

I corrected the pin 1 not connected to R3 net issue, it was stemming from eagle . i am attaching 4 screen shots ,showing LM7721 and LM7715 .  

please see the below schematic and screen shots . the highligted net lines shows which IC  iam selecting on both schematics n board.

Hi Sami,

Is there a reason you are using vias to go between pins 1 and 4 on IC1? It is okay to run a trace under the SMT part, but not close-spaced vias.

Just connect 4 and 1 on the top layer and save the cost of two two drill holes.

Otherwise, it looks good!

Some other layout comments:

The ground via on the bypass cap pad 2 on pin 6 of IC2 should probably come out towards the top instead of having the close spacing between the via and the V+ trace.

The closer the spacings, the more the board house will charge you. Same issue with the trace going to pad 2 of the 100 ohm output resistor on IC2 pin 8. The trace should come into the side of the pad, to prevent the "sliver".

Regards,

hi Paul!

good points .! applied your suggestions  please review

i have one question regarding the functionality of this circuit.  How does the P$SIG  gets the reference since the P$GND is not connected to

tthe physical ground ? 

regards

Sami

HI Sami,

Looks good.

The PH sensor is put in series with the 512mV reference voltage, so the output of the U2 buffer will be the reference voltage (P$GND) plus the sensor voltage.

Think of the sensor as a battery that changes it's voltage ±415mV depending on the PH concentration.

The U1 circuit generates the base 512mV reference voltage and the sensor voltage is added (or subtracted) from that, and U2 buffers the total voltage.

So the output of U2 will be 97mV (512mV - 415mV)  to 927mV (512mV + 415mV).

Regards,

hi Paul !

can I add the power plane on the top layer as follows  ? 

Hi Sami,

Yes. That is fine. Just make sure the input area is surrounded by the guard.

Also make sure you do not create "islands" in the ground plane. Make sure all the sections are connected.

Regards.

hi Paul!

i got the board made but its not working. its outputting a constant voltage of 2.55 volts at the output no matter in what kind of water I put   or even leave it open.  

can I send the board to you so you can test it in the lab environment ? 

regards

Sami