Preferred power supply connections?

dingebre wrote on Wed, 24 February 2010 21:57

This image kind of shows what I mean.

No, it shows a mess.  There is rotated text all over the place, labels

overlapping other labels and parts, and missing values.  If you don't care

about your design, there is no reason I should either.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

"Olin Lathrop" <eagle@embedinc.com> wrote in message

news:hm60oi$830$1@cheetah.cadsoft.de...

dingebre wrote on Wed, 24 February 2010 21:57

This image kind of shows what I mean.

 

No, it shows a mess.  There is rotated text all over the place, labels

overlapping other labels and parts, and missing values.  If you don't care

about your design, there is no reason I should either.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Olin,

This kind of response is completely inappropriate.  If you don't care then

don't bother responding.  Why even waste your time?

Unbelievable.

Terri

Olin wrote on Thu, 25 February 2010 07:16

dingebre wrote on Wed, 24 February 2010 21:57

This image kind of shows what I mean.

 

No, it shows a mess.  There is rotated text all over the place, labels

overlapping other labels and parts, and missing values.  If you don't

care about your design, there is no reason I should either.

Hi Olin, you're reading too much into the "design". This is not a real

schematic.

I'm only illustrating the power connections. I am showing the +/-15 volts

to the plug, and one way I was thinking to do the other power nets. I don't

even know if this design is electrically "real"

I only ask a little patience. I'm very new to using Eagle and want to learn

good habits. Would you maybe take a second look? I'd like some advice about

how to handle the power nets on the "real" circuits I'd like to work on.

Should I do it kind of like in that illustration? Use the supply library

+/- 15 for the plug and then a generic supply symbol to connect the +/-

supplies on the components? Or is there a better way?

Thanks for looking Olin.

David

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Terri Miller wrote on Thu, 25 February 2010 09:48

"Olin Lathrop" <eagle@embedinc.com[/email]> wrote in message

news:hm60oi$830$1@cheetah.cadsoft.de...[/email]

dingebre wrote on Wed, 24 February 2010 21:57

This image kind of shows what I mean.

 

No, it shows a mess.  There is rotated text all over the place,

labels

overlapping other labels and parts, and missing values.  If you

don't care

about your design, there is no reason I should either.

--

Browser access to CadSoft Support Forums at

http://www.eaglecentral.ca

 

Olin,

 

This kind of response is completely inappropriate.  If you don't care

then

don't bother responding.  Why even waste your time?

 

Unbelievable.

I agree Terry.  I've sent a PM to Olin about this.  You're not the only one

to complain.

James.

--

James Morrison  ~~~  Stratford Digital

email:  james@eaglecentral.ca

web: http://www.eaglecentral.ca

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

dingebre wrote on Wed, 24 February 2010 21:57

The schematic I am "capturing" are based on public domain circuits for

audio processing modules in a modular analog synthesizer. There are some

standard power connection schemes which I intend to follow consisting of

+/- 15 Vdc and ground. Typically, the +/- supplies go through a ferrite

bead and a couple of filtering capacitors before hitting the PCB's power

nets.

 

What is the best way to make a power net for the PCB components bcause

it is separated from the power input jack by the ferrite bead? If I

connect the connector pins to the supply +15 and -15 nets, I can't use

them on the PCB. So, what is the best net to use to PCB components to the

other side of the ferrite beads? Should use one of the other available

supply nets or make a unique power net?

 

I have played with different ways to do it, and they seem to work, but

as I'm new at this capture stuff, I'd like to know if there are standard

or preferred ways to accomplish this.

 

This image kind of shows what I mean.

Hi David,

There are a few ways to do it.  First, every signal name in EAGLE is

global.  So if you simply name a net to a signal name it will be connected

to any other net with the same name whether it looks like it or not.  So

watch yourself there.

So you have a pin connected to a ferrite that goes to a plane then you can

do a few things:

1)  name (and label) the net between the pin and the ferrite.  That can be

helpful.

2)  create a custom supply symbol that indicates  it's function.  This can

work too and can help with readability if that net goes somewhere else

(like a raw power bus).

My rule is that I should be able to tell 100% what is happening in the

schematic when I print it out.  If you have to use EAGLE itself (by using

the info command for instance) to figure out what is going on then the

schematic is incomplete.

I also have a preference for labels over spaghetti nets that are hard to

follow when printed out.  Hope that helps.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

email:  james@eaglecentral.ca

web: http://www.eaglecentral.ca

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

James Morrison wrote on Thu, 25 February 2010 09:52

dingebre wrote on Wed, 24 February 2010 21:57

The schematic I am "capturing" are based on public domain circuits

for audio processing modules in a modular analog synthesizer. There are

some standard power connection schemes which I intend to follow

consisting of +/- 15 Vdc and ground. Typically, the +/- supplies go

through a ferrite bead and a couple of filtering capacitors before

hitting the PCB's power nets.

 

What is the best way to make a power net for the PCB components

bcause it is separated from the power input jack by the ferrite bead?

If I connect the connector pins to the supply +15 and -15 nets, I can't

use them on the PCB. So, what is the best net to use to PCB components

to the other side of the ferrite beads? Should use one of the other

available supply nets or make a unique power net?

 

I have played with different ways to do it, and they seem to work,

but as I'm new at this capture stuff, I'd like to know if there are

standard or preferred ways to accomplish this.

 

This image kind of shows what I mean.

 

Hi David,

 

There are a few ways to do it.  First, every signal name in EAGLE is

global.  So if you simply name a net to a signal name it will be

connected to any other net with the same name whether it looks like it or

not.  So watch yourself there.

 

So you have a pin connected to a ferrite that goes to a plane then you

can do a few things:

 

1)  name (and label) the net between the pin and the ferrite.  That can

be helpful.

 

2)  create a custom supply symbol that indicates  it's function.  This

can work too and can help with readability if that net goes somewhere

else (like a raw power bus).

 

My rule is that I should be able to tell 100% what is happening in the

schematic when I print it out.  If you have to use EAGLE itself (by using

the info command for instance) to figure out what is going on then the

schematic is incomplete.

 

I also have a preference for labels over spaghetti nets that are hard

to follow when printed out.  Hope that helps.

 

Cheers,

 

James.

Yes, it helps a lot. Thanks James. In the software I have been using

(competing commercial application), it was a real chore to do this kind of

connection and I was a litte nervous as it seems so easy to do in Eagle

I wanted to make sure I wasn't missing something.

David

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

dingebre wrote on Thu, 25 February 2010 11:42

Hi Olin, you're reading too much into the "design". This is not a real

schematic.

 

I'm only illustrating the power connections.

It is still a good idea to keep in mind that neatness counts, especially

when you are presenting to others.  Some may look past that, but why allow

it to be a issue when it would only have taken a extra minute to make

things more readable?

Quote:

I only ask a little patience. I'm very new to using Eagle and want to

learn good habits. Would you maybe take a second look? I'd like some

advice about how to handle the power nets on the "real" circuits I'd like

to work on.

I don't use specific parts at all to label power nets.  I don't treat power

nets any different from other nets that are drawn in separate pieces,

although I've seen others use explicit power symbols commonly.  In Eagle,

nets in the schematic are automatically connected if they have the same

name.  To show airwires in a Eagle schematic, I name the nets and then use

DRAW LABEL to show the net name in the schematic.  It's important to use

DRAW LABEL instead of TEXT because DRAW LABEL shows the true net name as

Eagle understands it.  If you change the net name, the text drawn with DRAW

LABEL will automatically change.

For power nets I use names like "5V", "-12V", "BATT", or whatever I think

will be most descriptive in context of that schematic.  I also like to show

power connections on top, ground on the bottom, with signal from left to

right to the extent this can be reasonably done.  Keep in mind that the

schematic is not only to define the machine readable connections to Eagle,

but it is also the primary documentation of your circuit to humans.  As

such, neatness and clarity are very important considerations.

Quote:

Should I do it kind of like in that illustration? Use the supply

library  +/- 15 for the plug and then a generic supply symbol to connect

the +/- supplies on the components? Or is there a better way?

You'll probably find as many opinions as people.  There are several

reasonably "right" ways.  I've tried to explain what I do, but I recognize

there are other ways that others prefer.  As long as Eagle understands the

connections, there aren't hidden gotchas for making changes, and your

circuit is easy to understand from the schematic, then it's a acceptable

method.

You can take a look at http://www.embedinc.com/products/usbprog/eusb3.pdf

as a example of how I do things.  The first page is the main power supply.

Note all the named wires ending at the right side because the logical flow

is out from the power supply.  You can see various other places in the

schematic that connect to these power rails, usually coming in from the top

or left as a simple visual reference that the power is coming in instead of

being produced there.  Note that no explicit power symbols were used, just

named nets with carefully placed labels.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Olin wrote on Thu, 25 February 2010 12:49

dingebre wrote on Thu, 25 February 2010 11:42

Hi Olin, you're reading too much into the "design". This is not a

real schematic.

 

I'm only illustrating the power connections.

 

It is still a good idea to keep in mind that neatness counts,

especially when you are presenting to others.  Some may look past that,

but why allow it to be a issue when it would only have taken a extra

minute to make things more readable?

 

Quote:

I only ask a little patience. I'm very new to using Eagle and want

to learn good habits. Would you maybe take a second look? I'd like some

advice about how to handle the power nets on the "real" circuits I'd

like to work on.

 

I don't use specific parts at all to label power nets.  I don't treat

power nets any different from other nets that are drawn in separate

pieces, although I've seen others use explicit power symbols commonly.

In Eagle, nets in the schematic are automatically connected if they have

the same name.  To show airwires in a Eagle schematic, I name the nets

and then use DRAW LABEL to show the net name in the schematic.  It's

important to use DRAW LABEL instead of TEXT because DRAW LABEL shows the

true net name as Eagle understands it.  If you change the net name, the

text drawn with DRAW LABEL will automatically change.

 

For power nets I use names like "5V", "-12V", "BATT", or whatever I

think will be most descriptive in context of that schematic.  I also like

to show power connections on top, ground on the bottom, with signal from

left to right to the extent this can be reasonably done.  Keep in mind

that the schematic is not only to define the machine readable connections

to Eagle, but it is also the primary documentation of your circuit to

humans.  As such, neatness and clarity are very important

considerations.

 

Quote:

Should I do it kind of like in that illustration? Use the supply

library  +/- 15 for the plug and then a generic supply symbol to

connect the +/- supplies on the components? Or is there a better way?

 

You'll probably find as many opinions as people.  There are several

reasonably "right" ways.  I've tried to explain what I do, but I

recognize there are other ways that others prefer.  As long as Eagle

understands the connections, there aren't hidden gotchas for making

changes, and your circuit is easy to understand from the schematic, then

it's a acceptable method.

 

You can take a look at

http://www.embedinc.com/products/usbprog/eusb3.pdf as a example of how I

do things.  The first page is the main power supply.  Note all the named

wires ending at the right side because the logical flow is out from the

power supply.  You can see various other places in the schematic that

connect to these power rails, usually coming in from the top or left as a

simple visual reference that the power is coming in instead of being

produced there.  Note that no explicit power symbols were used, just

named nets with carefully placed labels.

Thanks Olin! I am used to a different commercial application which makes

things like this so difficult. Right now, the hardest part of my learning

curve is accepting how much simpler and more logical Eagle is compared to

what I have been using. I keep expecting Eagle to be much more cryptic...

Thanks for taking the time to share your thoughts. They are really helping

me get in the "Eagle" mindset. Next time I put up project, I'll clean it

up.

David

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Surprisingly nobody has mentioned EAGLE's gotcha with respect to power

supplies. EAGLE parts have named power supply pins that automatically

connect to the net of the same name. Furthermore, on many parts these

pins are hidden until you use the INVOKE command to bring them into the

schematic.

It becomes a problem when you try to use an opamp with say pin 4 defined

as -15V in the part. Add this part into your schematic and that

(invisible) pin is automatically connect to the net named -15V. If your

-15V net is called VEE or VSS, no connection. Guess what happens when

one part has a pin named VCC and another part has a pin named +15V and

you need to connect both to the same +12V power supply rail...

I don't like these implicit nets at all and I do not use them, but they

are found all the time in the EAGLE library parts. I believe the newer

versions of EAGLE may have an option to disable this behavior. ( I still

use v4 ). Look in the EAGLE help for SUPPLY and POWER directions for

pins to understand this a little better.

I do use power supply symbols and I also frequently label the nets like

Olin does. I document all power supply connections in the schematic

along with their bypass caps, and never use the implicit ones.

Gary Gofstein wrote on Thu, 25 February 2010 18:56

Surprisingly nobody has mentioned EAGLE's gotcha with respect to power

 

supplies. EAGLE parts have named power supply pins that automatically

 

connect to the net of the same name. Furthermore, on many parts these

pins are hidden until you use the INVOKE command to bring them into the

 

schematic.

 

It becomes a problem when you try to use an opamp with say pin 4

defined

as -15V in the part. Add this part into your schematic and that

(invisible) pin is automatically connect to the net named -15V. If your

 

-15V net is called VEE or VSS, no connection. Guess what happens when

one part has a pin named VCC and another part has a pin named +15V and

 

you need to connect both to the same +12V power supply rail...

 

I don't like these implicit nets at all and I do not use them, but they

 

are found all the time in the EAGLE library parts. I believe the newer

 

versions of EAGLE may have an option to disable this behavior. ( I

still

use v4 ). Look in the EAGLE help for SUPPLY and POWER directions for

pins to understand this a little better.

 

I do use power supply symbols and I also frequently label the nets like

 

Olin does. I document all power supply connections in the schematic

along with their bypass caps, and never use the implicit ones.

Excellent point. I hadn't given that much thought.

David

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca