Linear power supply project

[Therm Mr.]

Thanks pqass that is very helpful info. I did download KiCad I am about half way through the drawing. So it is pretty intuitive. I stopped to resolve the below issue before I get ahead of myself and have to backtrack. The one thing I did notice is the library is missing many components. Like the tip142 not being in there. It does not seem like a big deal because I can use others as a generic symbol. Seems like it would only be a problem if I wanted to print the parts list, which I don't plan on doing. But I do like the program so far. I'll post the drawing for any critique when I am done.

At the very end of the drawing there are two caps, c3 and c4 that are deleted in the 3610. Now wiring a direct by-pass looks like it would create a dead short between output positive, output negative and ground. My thoughts are to eliminate the line between ground and output positive but maintain the line between output negative and ground. Am I thinking correctly here?

andrewtaylor thanks for the advice and I am all in on the 3610 build. The other schematics will be good learning tools and references in the future.  Also I found an app Electronics Engineer Helper. Lots of good tools to help. I use a Mac so good software is not as prolific as on windows.

Kleinstein I do plan on working a little with both TINA and LTspice to evaluate them for use. One can never have too many tools.

Therm

[Kleinstein]

Tina and LTspice are about comparable - usually no real need to have both. There is still some learning curve for the UI.

In the original plan one could get away without C4 or or C5. They both get a capacitive link to mains ground, mainly for RFI purposes. Because of RF oddities (even wires can have an effect) it can still make sense to have them both.

A capacitor like C3 at the output is essential and the capacitance (with details like ESR) here is an important point in the design. One may even consider more than 1 capacitor in place of C3, like a small (e.g. 100 nF range) film or ceramic and a larger electrolytic (e.g. 100 µF, possibly more) that acts as capacitor with some ESR. The compensation is a bit similar to classic LDO regulators and similar to these the regulator can be a bit picky about the output capacitor(s).

The plan has different ground symbols and it is correct to have the positive output connected to the +S ground that is also the center of the regulator supply.

[pqass]

Thanks pqass that is very helpful info. I did download KiCad I am about half way through the drawing. So it is pretty intuitive. I stopped to resolve the below issue before I get ahead of myself and have to backtrack. The one thing I did notice is the library is missing many components. Like the tip142 not being in there. It does not seem like a big deal because I can use others as a generic symbol. Seems like it would only be a problem if I wanted to print the parts list, which I don't plan on doing. But I do like the program so far. I'll post the drawing for any critique when I am done.

At the very end of the drawing there are two caps, c3 and c4 that are deleted in the 3610. Now wiring a direct by-pass looks like it would create a dead short between output positive, output negative and ground. My thoughts are to eliminate the line between ground and output positive but maintain the line between output negative and ground. Am I thinking correctly here?

With Kicad, you typically won't find specific part numbers in the library.  So when adding to the schematic editor choose generic symbols like "Q_NPN_Darlington_BCE" for TIP142; making sure the pin numbering 1,2,3 corresponds to your actual part ordering for B,C,E.  Then change the value of the highlighted symbol via mouse right button > Edit Value item to "TIP142".   After you're done with the schematic editor, run the Footprint Assignment Tool to select the correct footprint for every part.  In your case, for TIP142, you can choose "Package_TO_SOT_THT:TO-247-3_Horizontal_TabUp" if you wish to sandwich the part horizontally between heatsink and PCB.

In the case of C5 and C4... don't take my earlier advice too literally ("non-applicable components were removed or replaced with a short").  Context is important.  The E3612A has high-voltage outputs (120VDC) and as such will have Y-rated safety caps to earth ground (the pitchfork symbol, aka the 3rd mains prong).  So, no, don't short C5 and C4; just remove them entirely.  You will find all these lab supplies have the earth ground available on the front face-plate giving the option to the user to tie the positive or negative output post to it, or not; leaving the output "floating" WRT earth (ie galvanically isolated).

Try to understand the purpose of each component.
Is the component required for core functionality or does it support a secondary feature (eg. CV, CC, voltage, current display)?

[Solder_Junkie]

Kleinstein I do plan on working a little with both TINA and LTspice to evaluate them for use. One can never have too many tools.

Therm

I use both, LTspice is excellent if you are using their devices, but I find the user interface of Tina "better" for most uses. I guess it depends on what you become used to.

While I have a copy of KiCad, I find it frustrating to use and much prefer Sprint Layout: https://www.electronic-software-shop.com/lng/en/electronic-software/sprint-layout-60.html but as with Tina vs LTspice, it depends on your preference. I have made a lot of boards, both home etched and made by JLCPCB, using Sprint Layout.

SJ

[Therm Mr.]

KiCad is quite impressive it has a few quirks but is easy to learn and use and you can't beat the price. The symbols are not scalable so they are probably not vector drawings. You guys really hooked me up good with that one. KiCad is pretty functional for a free program. I expect Ltspice/TINA will be good too.

This is the drawing I did in KiCad. I left everything in for now ie, display power and CC/CV circuits. I wanted to have a good representation of what a 3610a circuit looks like, not a multi unit circuit. Also I used three transformers that just for drawing purposes for now I will figure that out as I go. I found some DVM modules at Mouser made by Murata, that are loop powered by the input voltage and current. They would eliminate the power supply circuit. I need to investigate that a bit more though.

I will admit the whole V- V+ and floating ground vs earth ground thing has me a bit confused. Also +S is a giant WTF. But its only a matter of time before it starts to sink in. Right now the connector J1 has two number threes but it won't be hard to sort out once I pick a display. Let me know if you see anything I messed up.

Thanks again Gents
Therm

Found a few errors in the original file so I deleted and re-uploaded.

[Solder_Junkie]

Wow, that diagram is impressive! Well done getting that far in KiCad. The harder part is turning it into a print board layout 😂

SJ

[Therm Mr.]

With Kicad, you typically won't find specific part numbers in the library.  So when adding to the schematic editor choose generic symbols like "Q_NPN_Darlington_BCE" for TIP142; making sure the pin numbering 1,2,3 corresponds to your actual part ordering for B,C,E.  Then change the value of the highlighted symbol via mouse right button > Edit Value item to "TIP142".   After you're done with the schematic editor, run the Footprint Assignment Tool to select the correct footprint for every part.  In your case, for TIP142, you can choose "Package_TO_SOT_THT:TO-247-3_Horizontal_TabUp" if you wish to sandwich the part horizontally between heatsink and PCB.

pqass
Try to understand the purpose of each component.
Is the component required for core functionality or does it support a secondary feature (eg. CV, CC, voltage, current display)?

I was finding mistakes the more and more I looked over the circuit drawing. I was trying to make sure everything was right before I tried to run the foot print assignment tool. Just to try it out, not because I have finalized anything.  I was editing because there were some lines drawn over the top of the symbol that I did not put there. U4 and U5 which of both have A and B sections and the A and B were doubling and I was trying to figure out why. So I went back and re-read the above several times trying to look for answers. Thats when it hit me and I started to understand what you were saying.

So now I am wondering if I need to go back and change some of the components I inserted not just edit them. I am going to post to pics in this post to see if you can confirm that I do now understand your post.

The pics are of Q 1 and 3. I changed the pins on Q 3 to match the transistor in the other picture. Did I do that correctly?

When I was putting in U2, 4 and 5 I just picked the symbols at random if they matched the numbering I needed for the drawing. If not I edited them to match. The components in the parts list did not have matches in the symbol library. Will that screw me later when I go to the footprint assignment tool? Better to correct it now than later.

Where can I cross reference obsolete parts to find the modern replacements?

Kleinstein good info on the caps thanks.

I just noticed that Q3 changed to Q2. I re-uploaded to fix. I have had this happen on many things while working is it me or the program just glitching?


Thanks
Therm

[pqass]

The pics are of Q 1 and 3. I changed the pins on Q 3 to match the transistor in the other picture. Did I do that correctly?

Yes. Q1 should look like Q2 in your attachment. That is, for the TIP142 part, pin 1=B, 2=C, 3=E.

If not I edited them to match.

Not sure what you mean.  I hope you didn't change the symbol via the Symbol Editor.  That shouldn't be necessary for the complexity in this schematic.  The haystack is pretty big so sometimes it's hard to find an appropriate generic symbol for your needs.

Where can I cross reference obsolete parts to find the modern replacements?

LF411 and LF442 both have generic footprints; 1 opamp, and 2 opamp packages, respectively. If you implement IC sockets, you can try many specific devices during testing.  Unfortunately, there are lots of modern parts to choose from which usually requires you to read the datasheet on the old part and compare it to more common modern parts.  I'm not aware of a specific xref list except to say that my 2nd Ed Art of Electronics says LF411=jellybean.  Digikey also still sells the LF411, however, the LF442 is listed as obsolete though shows substitutes (not sure of the value, worth checking though).

LM336BZ5.0 can be substituted for with a TL431 + two 10K divider resistors.

LM393 is still readily available.

[Therm Mr.]

Yes I went into the editor and edited till I got a match. Is there a way to reload that library?   

[pqass]

You should have seen a message (just under the icons): "Editing symbol ? from schematic.  Saving will update the schematic only."

So delete the symbol from your schematic and Add the generic one back in.
The edited symbol might still be in a cache in your local directory so don't re-select it as it may be listed as most recent in the Add list.

[Therm Mr.]

Thank you, That is exactly what I saw. Your help is very much appreciated.

Therm

[pqass]

I found some DVM modules at Mouser made by Murata, that are loop powered by the input voltage and current. They would eliminate the power supply circuit. I need to investigate that a bit more though.

I will admit the whole V- V+ and floating ground vs earth ground thing has me a bit confused. Also +S is a giant WTF. But its only a matter of time before it starts to sink in. Right now the connector J1 has two number threes but it won't be hard to sort out once I pick a display. Let me know if you see anything I messed up.

The thing with lab power supplies is that you can dial the output down to 0V.  So you can't really power the voltmeter with the output voltage as it will cut-out at some point as you dial down.  Also, ammeter modules include their own shunt (another low value resistor like R2) which will lower the output by the burden voltage.
In the case of the E3610A R2=0.1ohm, therefore a 1A current will produce 100mV and a reading of 1000 on a 0-200mV full-scale 3-1/2 digit voltmeter.
In the case of the E3611A R2=0.2ohm, therefore a 1A current will produce 200mV but to use the same voltmeter, R11+R12 (10K+10K) divider is used to cut that in half.
So the purpose of the R11+R12 divider is to adapt the shunt to the voltmeter selected (as ammeters are just voltmeters measuring shunts).
Same for R18+R17; to adapt the output voltage range to the voltmeter selected (showing the output voltage reading to the user).

Yes, I saw the pin3 referenced twice mistake too.




Now, onto a critique of your schematic...

Wires should go from symbol pin to symbol pin; don't just end wires as it will fail DRC and will be a mess going forward into the PCB layout stage.  Unused pins should have the "x" (no connection) flag attached (see right icon bar).

Don't mimic switches with wires; there are many switch symbols. Search under the "Switch" category in the Add symbol popup or search for "SPST", "DPDT", etc. in the search bar.  It's a big haystack. For example, if you can't find one like "SP7T", open "SW_SP3T", edit it, create/save-as to your own library for future projects.

I find HPs schematic hard to follow with all the long wires going between sub-circuits.  I like to isolate bite-sized parts (but not go too microscopic) and connect them through global or local labels. See what others have done on the Internet to get a feel for it.

Use the power symbols; Add symbol from the "Power" category or ⏚ on right icon bar. Don't just end wires with "+12V" or "[+S]" text. If you have two rails that are the same voltage but should be isolated, then select a different power symbol (eg. "+5V", "+5VD").  Also, google "kicad PWR_FLAG".

[Not in yours but] most schematic readers expect inputs on the left, outputs on the right.  Similarly, positive power is ordered above GND and negative power below GND.

Once you think you're done with the schematic,
a. either manually change all reference designators (eg. "Q?", "U?") to match HPs schematic or use the Annotate Schematic popup to (randomly) assign them for you. 
b. Then run rules check via Electrical Rules Checker popup. 
c. Then call Assign Footprints popup to select footprints for each symbol. 
d. Only then you can proceed to the PCB layout editor.


Attached, you will find my take on a re-written version of the the E3610A. Your style may be different and that's okay.
a. I've purposely cleared all reference designators to "?" and kept the default for the symbol value field to show the generic symbol chosen.  I also re-organized and separated the sub-circuits into functional chunks which I believe are easier to read/understand.
b. Op amp GND (▽) and "+S" label are attached at the positive output post.
c. I use the protective earth symbol for the 3rd plug prong which is isolated from op amp GND above.  Unfortunately, the stupid plug symbol has a ⏚ which is confusing with PE symbol attached to the pin. I/you should just make your own library version without the ⏚ lineart.
d. +5V in the original isn't really used as a power rail.  It's really a stable +5V reference so I made it a label instead of using a power symbol.
e. Notice the display power uses +5VD/GNDD which is isolated from any other rail.
f. I've substituted a TL431+2*10K for the LM336.
g. I've used connectors for J1 and the output posts. As far as I'm aware, you can't split a single connector; distributing the pins over the schematic like HP did for J1. It must be a single n-way connector with wires or labels attached.

That's all for now.

[Therm Mr.]

That is all? That is a mind and a half full.

I do already have some questions but let me digest that all a for bit first. While drawing the HP version I learned a lot just from the process. As I wrestled my way through it and KiCad together, I though I might go into info overload. Yet I lived through it. That drawing was a little intense to flow through. By breaking it up into bite size nuggets you definitely have made it little more friendly to the brain for sure. That must have been a bunch of work.

I will probably read that last post 10 times before I comprehend the better part of it. I can't even begin explain how much I appreciate the education. I started a spread sheet for a parts list that I have been working on with this. I have even got a couple of saved carts with parts at some suppliers. I want to get these parts so I can start building some circuits for testing. I just have to be careful not to get ahead of myself.

Getting some build time on the bench with a DMM and a scope will hopefully pull all this random stuff rattling in my head together.

Thanks

Therm

PS Thanks for the critique. It will certainly help me improve my drawings.

[Therm Mr.]

The thing with lab power supplies is that you can dial the output down to 0V.  So you can't really power the voltmeter with the output voltage as it will cut-out at some point as you dial down.

Thinking about it that is pretty much a no brainer. You can’t power a display at zero volts. Sometimes I wonder about myself.

Wires should go from symbol pin to symbol pin; don't just end wires as it will fail DRC and will be a mess going forward into the PCB layout stage.  Unused pins should have the "x" (no connection) flag attached (see right icon bar).

This is very helpful I have been deleting unused pins or picking the wrong symbol to try and match the HP drawing. It would have become a big problem later. Thanks

Don't mimic switches with wires; there are many switch symbols. Search under the "Switch" category in the Add symbol popup or search for "SPST", "DPDT", etc. in the search bar.  It's a big haystack. For example, if you can't find one like "SP7T", open "SW_SP3T", edit it, create/save-as to your own library for future projects.

Noted and I will make the changes. When using a created library do you need to switch back and forth between libraries to use them? Or how does that work?

I find HPs schematic hard to follow with all the long wires going between sub-circuits.  I like to isolate bite-sized parts (but not go too microscopic) and connect them through global or local labels. See what others have done on the Internet to get a feel for it.

I find HPs schematic a bit quirky too. I do understand the circuitry much much better the way you drew it. But I lose the big picture in the little bits and need to see the circuit whole and connected to visualize the and understand project. If thats make any sense.

Use the power symbols; Add symbol from the "Power" category or ⏚ on right icon bar. Don't just end wires with "+12V" or "[+S]" text. If you have two rails that are the same voltage but should be isolated, then select a different power symbol (eg. "+5V", "+5VD").  Also, google "kicad PWR_FLAG".

I think I am starting to get this. I am still a bit confused by all the different power rails and grounds and the reasons for them. My understanding of this part of it is getting better all the time. I imagine at some point I will have that epiphany moment.

Once you think you're done with the schematic,
a. either manually change all reference designators (eg. "Q?", "U?") to match HPs schematic or use the Annotate Schematic popup to (randomly) assign them for you. 
b. Then run rules check via Electrical Rules Checker popup. 
c. Then call Assign Footprints popup to select footprints for each symbol. 
d. Only then you can proceed to the PCB layout editor.

I have a ways to go before I get here. I have been putting HPs designators in because it helps me match to their parts list. So are you saying redraw and just leave them blank for now?

Attached, you will find my take on a re-written version of the the E3610A. Your style may be different and that's okay.
a. I've purposely cleared all reference designators to "?" and kept the default for the symbol value field to show the generic symbol chosen.  I also re-organized and separated the sub-circuits into functional chunks which I believe are easier to read/understand.

They are much easier to understand. How do the global/local labels work when running the rules and PCB layout? Also where can I find out about using them and where to create them.

b. Op amp GND (▽) and "+S" label are attached at the positive output post.

Noted

c. I use the protective earth symbol for the 3rd plug prong which is isolated from op amp GND above.  Unfortunately, the stupid plug symbol has a ⏚ which is confusing with PE symbol attached to the pin. I/you should just make your own library version without the ⏚ lineart.

I wondered why you did that what is the difference between the two?

d. +5V in the original isn't really used as a power rail.  It's really a stable +5V reference so I made it a label instead of using a power symbol.

? Reference for what? This has me confused.

e. Notice the display power uses +5VD/GNDD which is isolated from any other rail.

Noted this I understand.

f. I've substituted a TL431+2*10K for the LM336.

In HPs drawing is this a mistake? The LM336 has no adjust wire attached what exactly is this doing?

g. I've used connectors for J1 and the output posts. As far as I'm aware, you can't split a single connector; distributing the pins over the schematic like HP did for J1. It must be a single n-way connector with wires or labels attached.

I liked how you did that. The actual HP device has just such a connector. When I looked it up in the symbol library it did not have the yellow rectangle around it. Thats when I figured out you must have edited and created it. Then I did the same it was a good lesson by itself.

[pqass]

When using a created library do you need to switch back and forth between libraries to use them? Or how does that work?

No.
You can create a library from the Symbol Editor menu: File > New Library...   Save to <home>/Schematic/lib/<library name> 
Then in the Schematic Editor, add it to the bottom of menu: Preferences > Manage Symbol Libraries...
It will show up as an expandable category on the Add (symbol) popup.  And the content is searchable via search bar.

But I lose the big picture in the little bits and need to see the circuit whole and connected to visualize the and understand project.

I agree, too fine a sub-circuit breakdown leads to disjointed puzzle pieces.  That's where placement of the pieces and label names visually helps (flow from left -> right, top -> bottom).  You can always create a high-level function diagram in a corner.  Or if too elaborate for one large sheet, use hierarchical sheets. BTW: you can change to a larger sheet via File > Page Settings then scale down to a US Letter when printing to PDF.

I am still a bit confused by all the different power rails and grounds and the reasons for them.

The display power is isolated from the rest of the circuit because ICL7107-based 3-1/2 digit voltmeters need that; can't be galvanically attached to the thing they're measuring.
The op-amp power needs to be isolated because the only point of its attachment will be its GND with the +OUTPUT post.  Why? A:Because the opamps need to change the voltage on the base of the darlingtons relative to their emitters (which are two low-value resistors away from +OUTPUT) and don't have to take into consideration the variable output voltage setting. Like a bird on wire; it doesn't know it's at many KVs relative to earth.

I have been putting HPs designators in because it helps me match to their parts list. So are you saying redraw and just leave them blank for now?

No. I left them ? because (1) I didn't want to distract from calling them something else (by auto generating) vs. the HP drawing., and (2) it's more work to match HPs drawing.  The intent of my drawing is to show sub-circuit breakdown and layout, not do it for you.

How do the global/local labels work when running the rules and PCB layout? Also where can I find out about using them and where to create them.

Global labels connect wires over separate pages; local labels don't leave the page.  Find them on the first two "A"s on the right icon bar.

I wondered why you did that what is the difference between the two? [GND vs PE]

Ground is such an over-loaded word!  To electronic engineers it means 0V; what other wires are measured from.  To power/electrical engineers it means the planet.    Sometimes electronic engineers need to reference both so call one GND/0V the other PE (protective earth).  In the case of this power supply, a feature is that it is isolated (like it were a battery) which allows us to stack several in series.  If one output was attached to PE, it may cause shorts in the thing you're powering or other non-isolated power supplies.  Hence, leave it to the user to tie to PE at the front post if he so wishes.

[RE +5V Reference] ? Reference for what? This has me confused.

A power source (vs reference) is meant to supply energy to the circuit. It may be a regulated voltage but isn't expected to be very precise; can vary +/-5% in most cases.  A reference is meant to be very stable so it can be used to measure with. In this case, +5V is used to set up the desired current and voltage settings.  It's not meant to supply, say, the op-amp power pins.

In HPs drawing is this a mistake? The LM336 has no adjust wire attached what exactly is this doing?

No, HPs drawing isn't a mistake. the LM336 is a fixed 5V zener; adjustment not possible.  I substituted it for a TL431 because I had one for the repair to my E3611A and wanted to show it was a viable substitute.  You can go with the LM336 if you wish.

The actual HP device has just such a connector. When I looked it up in the symbol library it did not have the yellow rectangle around it. That's when I figured out you must have edited and created it.

Scroll-down, it's there under "Connector_Generic" category.  I didn't use any home-made symbols.  All of them are out-of-box.  That's why I didn't change their default value to a meaningful name.

[Kleinstein]

Instead of a 431 plus 2 resistors one can also use 2 x TL431 in series for slightly lower noise.

The ICL7107 in principle has a differential input. If you build your own PCB for the converter one can power it from the same supply (with extra regulators from the +-12 V) as the regulator part. It is only the ready made panel meter modules that usually have the negative side linked to the supply.

[Therm Mr.]

pqass
That answers alot of questions and the ground explanation was an eyeopener.  I wondered why there was a ground and neg terminal on the front panel. So the ground is earth or protective the negative is just isolated to the device. Is that correct?

What is S+ why a plus if a ground?

The power flag is just to let the program know there will be power on the circuit? Correct? Why does the display and reference need it but not the power circuit?

I think I figured out the labels looking at the properties of yours. I thought one would be an output and one and input but yours were both inputs. ie VMETER were both inputs. I first thought the circuit side would be an output and the plug side an input. So what determines the shape?

Kleinstein good to know about the lower noise.

So the ICL7107 PCB can be designed to eliminate the additional supply without sacrificing device performance? Is that what you are saying?

[Kleinstein]

Yes one can design a ICL7106/7 circuit that does not need an extra supply just for the display. Just use the differential input of the ICL7107 (most panel meters tie the neg side to the supply or a fixed ref. voltage and for this reason need the separate supply). No complicated circuit (maybe even patch / hack a standard panel meter) needed and essentially the same performance. One may need extra voltage regulators (e.g. +-5 V).

The power flags are for the design rule checks. Some of the symbols like ground or +12 V have an implicite power flag.


The actual DC supply is normally isolated from main ground (PE). The PE terminal is there to allow for the connection (usually to the neg side, but could be the positive side too) by the user.

[Therm Mr.]

The advice and help I have received has led to many improvements. I think I am getting closer to a doable plan. I am sure its not perfect yet but I will get there. I have a bunch of stuff to do for most of the rest of the week. I will be chomping at the bit to get back to this.

Here is the latest rendition. Thanks you guys great.

Therm

[Kleinstein]

The signal to the current error amplifier is wrong: it should not be - output, but more Tp1. The curretn control signal is also not reaching the regulator.

The regulator supply also has a mistake: ground and the neg side of the rectifier are swaped. There is also a connection missing from the regulator GND pins.

[pqass]

"... the negative is just isolated to the device. "

Yes the "-" (center) post is the negative to the "+" (left) post; like an isolated, variable "battery".  The "⟂" (right) post is the PE connected to the 3rd plug prong, usually the metal case (but not on the E361xA as they are plastic), the transformer iron core (in case a winding touches/burns through to it), and the back metal heatsink.
Without an PE wire, if you were touching the outside metal parts and the an internal mains wire touched it, energy can flow through you to the concrete floor.  All mains power has the neutral line attached to the physical earth (via rod) at the power plant and every street pole. It's a shorter path (less resistance) to trip the breaker through the PE wire than you.

What is +S why a plus if a ground?

I have no clue why HP called it that. I just thought I would do the same for continuity.  I could have used the GND (▽) symbol everywhere instead but I wanted to convey that all those places that use +S>--- label should be directly attached to the +OUTPUT post (like a "star") since many times GND is just a "pour" over the whole board.

The PWR_FLAG is only a Kicad thing. It's not relevant to the circuit itself. In Kicad, symbol pins have defined purposes: input, output, bi-dir, tri-state, ..., and power in/out.  Some symbols have their power pins hidden and kicad automatically connects them to wires (nets) of the same name. DRC complains otherwise.   The reference doesn't need a PWR_FLAG because it's only going into (resistor) symbols that have pins defined as "passive" or "input" (not "power in").
BTW: there still is a DRC warning and error in my version. The warning says there are two names for the same net (GND and +S) and it chose +S. The error says I need a PWR_FLAG on the PE wire. But PE is a safety and not a full-time power wire. I ignored the error.

Labels don't really have a direction, however, the way I draw them (my convention) is a hint. If attached on the left of the wire, it's an input. If attached to the right of the wire it's an output. eg.  VMETER>--- is input, ---<VMETER is output.  I did the latter with the panel meter resistor dividers and the former with pin 4 on the 9-way connector. 

So the ICL7107 PCB can be designed to eliminate the additional supply without sacrificing device performance? Is that what you are saying?

WRT the ICL7106/7... most of the panel meters you can buy will probably be based on this chip but it depends on how they breakout the power and sense inputs. Some panel meters "add value" by just providing one pair for power and sense; good for up to 100V.  But that won't help you due to reasons noted in my reply#36.  I have personal experience with this panel meter (used in one of my projects) but it wouldn't work correctly/bad readings if the negative sense was connected to the negative supply (though it should work according to Kleinstein). Luckily
after some research, I ended up creating a capacitor-isolated supply based on this (bottom of page; FYI: without lower inverter as it causes glitches). But this won't work for LED displays due much higher current requirement; LCD version only needed <5mA@9V which can be created with a charge-pump PS.

Also, I'm pretty sure the right LED display (showing current on the E361xA) has the sign and most significant digit (+1, -1) removed (just showing 3 whole least sig. digits). I know this because CREF output is a variable negative quantity from 0 to -6V and CREF4METER being 5% of that corresponds to 0.00..3.00A as seen on the display.  However, CMETER being from the left of the (R2) shunt will be positive. But both CMETER and CREF4METER are switched by a momentary SPST into the same +V meter input to the 9-way connector; -V meter being +S/GND.  You won't have that luxury if you buy an off-the-shelf meter.

Wait 'till you get to understanding how the voltage and current regulation works. 
Hint: negative feedback going from each error amp through the diode-OR logic and then the darlingtons back to the error amps.

[Kleinstein]

WRT the ICL7106/7... most of the panel meters you can buy will probably be based on this chip but it depends on how they breakout the power and sense inputs. Some panel meters "add value" by just providing one pair for power and sense; good for up to 100V.  But that won't help you due to reasons noted in my reply#36.  I have personal experience with this panel meter (used in one of my projects) but it wouldn't work correctly/bad readings if the negative sense was connected to the negative supply (though it should work according to Kleinstein). Luckily

Most panel meter boards need a separate supply, as they have the negative input of the ICL7107 chip tied to the the comm pin (internal reference). In a few cases it my ay be linked to supply GND - this would kind of work but could add some offset from ground current and the sign would be wrong.  Without this link the ICL7107 has a true differental input and could used a supply (e.g. +-5 V) relative to +S. This supply could than use the same transformer as the OP-amps.  To get the right sign one would have the + input of the ICL7107 at the +S side of the shunt and use the negative input of the ICL7107 for the voltage divider or other side of the shunt.

[Therm Mr.]

The signal to the current error amplifier is wrong: it should not be - output, but more Tp1. The curretn control signal is also not reaching the regulator.

The regulator supply also has a mistake: ground and the neg side of the rectifier are swaped.

I should have caught that thanks. I think this fixes it.

I don't understand this part, what is missing? "There is also a connection missing from the regulator GND pins".

Nevermind I spoke soon I think this is it correct?

[pqass]

See attachment regarding these issues.
A: Fuse on wrong side of transformer.
B: Center-tap of transformer is GND and the negative of the diode bridge goes to the 7912.  You have them swapped.
C: 7912 pinout is wrong.
D: Diode on the loose.
E: If these two diodes represent two TL431s then use the correct symbol for TL431 and connect their adjustment pin to their cathode (to program for 2.5V).
F: Use the +S label instead of text.
G: +/- opamp inputs are swapped.
H: Missing junction with +S/+OUTPUT wire (needed for R18 at least).  Maybe remove R11 (not populated on the E3610A) and R12 entirely; just attach SW1 pin 1 to left side of R2.
I: Wire from R23 goes to -OUTPUT when it should go to center of R27+R34 divider. Also, R34 looks shorted; wire between pins. FYI: R26+R34 divider is a bit of joke from HP because of the ridiculously tiny 1R/500K ratio. They should've just attached R23 to left-side of R2 and removed R27 and R34 entirely.
J: Don't use broken wires; use a jumper symbol like "Jumper_2_Open".
K: It looks like you removed defined pin 3 when you edited this symbol; looks like lineart just ends. If the PE symbol doesn't attach to a defined pin then DRC will report an error.



WRT the ICL7107... after reading this AppNote several times, it basically says:
you need to supply bipolar power (V+=+5V, GND=0V, V-=-5V), otherwise you'll have to offset the negative sense input via opamp; can't tie it to GND if powered via single-supply.   With a purchased panel meter, you don't know if they are generating their own negative supply (and is likely not).  Hence the need for an isolated supply for the panel meters.

[Therm Mr.]

pqass and Kleinstein, Thank you for those corrections. Most of what you all pointed out I should have caught. I think I made the corrections properly. If not let me know. Its good to have fresh experienced eyes look sometimes. I have to look in minute detail to find errors, where your eyes see them it seems more instinctively.

pqass I had changed the jumper (JP1) before you mentioned it. I just put x like you said it should be for unconnected wires. But I was thinking couldn't I just eliminate the JP1 wire, it does nothing now?

Also I added power symbols to the outputs is that correct?