Can a generic symbol (sup) be created?

Hi,

I guess part two of this question is how do you connect nets between multiple schematic sheets.

If you run a net and give them both the same name, the ERC says "Segment of net X has no visual connection.  Surely there must be a right way to do this between multiple sheets.

Thanks,

Alan

On Thu, 2 Sep 2010, alank2 wrote to us saying :

>If you run a net and give them both the same name, the ERC says

>"Segment of net X has no visual connection.  Surely there must be a

>right way to do this between multiple sheets.

Is that just a net from nowhere to nowhere? Because the way to connect

nets between sheets is simply to give them the same name. As long as the

net connects to at least one pin of at least one part on each sheet it

appears on, then you shouldn't get that error. And if it doesn't then

why is it even on that sheet?

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of     | If you believe Satan is found in pop can I

this message are    | suggest you stop drinking it.

purely my opinion.  |    - Dave Hyden, uk.r.c,

Don't believe a     |    re: "Stairway to Heaven"

word.               |

Hi,

If I put a single part on each sheet and then add a net to one pin on each part and then use the name to join the two nets together, the warning still comes up.  Do you put something at the end of the net when using multiple sheets and a net goes only from one pin on one sheet to one pin on another?

The way Eagle handles these "unwired" but connected nets seems so much harder than it needs to be.  I don't know why they don't just have a single pin symbol you add and then tell it which net it goes to...

Thanks,

Alan

alank2 wrote:

>If I put a single part on each sheet and then add a net to one pin on each part and then use the name

to join the two nets together, the warning still comes up.  Do you put something at the end of the net

when using multiple sheets and a net goes only from one pin on one sheet to one pin on another?

help label

>The way Eagle handles these "unwired" but connected nets seems so much harder than it needs to be.

I don't know why they don't just have a single pin symbol you add and then tell it which net it goes to...

I rather like this warning. It reminds me to put labels on nets that

are present on more than one sheet.

--

Lorenz

"alank2" <communitymanager@premierfarnell.com> wrote in message

news:245768910.5331283470906554.JavaMail.jive@flcspu-csapp-01.premierfarnell.com...

Hi,

>

If I put a single part on each sheet and then add a net to one pin on each

part and then use the name to join the two nets together, the warning

still comes up. Do you put something at the end of the net when using

multiple sheets and a net goes only from one pin on one sheet to one pin

on another?

>

The way Eagle handles these "unwired" but connected nets seems so much

harder than it needs to be. I don't know why they don't just have a single

pin symbol you add and then tell it which net it goes to...

>

Thanks,

>

Alan

>

why do you think "xref" was invented?

Hi,

Thanks guys, the label and xref were exactly what I needed to figure out how to use.  I just didn't know how they worked.

Alan

Hi,

So, what is the difference between using something like a supply +5V from the library vs. just drawing a net and naming it +5V and giving it an xref ?

Thanks,

Alan

>

So, what is the difference between using something like a supply +5V from

the library vs. just drawing a net and naming it +5V and giving it an xref

?

>

Thanks,

>

You can't give supply nets arbitrary names with supply symbols as

implemented as a library component without overwriting the resulting power

net name. When you drop a power symbol on a sheet and connect it to a net,

it uses the name assigned to the SYMBOL PIN in the library SYMBOL (not the

device name) as the new power net name to assign in the schematic.

I can't tell you how many drawings folks have sent me with screwed up power

symbols, nets, etc due to this. For instance, if you overwrite a supply

symbol net name and then use the COPYcommand to duplicate that power symbol

and connect it to a new net, the new net will have the original name that

was assigned to the pin in the SYMBOL rather than the net it was currently

assigned to. I see lots of drawings where beginners do this and have power

nets all goofed up and/or not connected properly. I've seen lots of

improperly created power symbols with the pin name different from the

symbol/device name which can really cause havoc in a drawing with power nets

all tied incorrectly to each other.

In other systems, like Altium, the power symbol is a native object in the

schematic and you can give it any arbitrary name you like when you add a

power symbol. Your limited to a few power symbol types (like a t-bar, circle

or arrow), but I like this for consistency reasons. If you duplicate the

symbol and connect it to another net, then  it uses the arbitrary name

assigned to that symbol instance (rather than using the original name from a

lib object). None of this business of  "the power symbol net name was

overwritten" warnings or confusion exists.

It wouldn't be that big of a deal to add a native power symbol object in the

schematic editor. But, converting all the old drawings that use the lib

power symbols would be a little bit of a conversion headache.  I'd be

perfectly happy to see these gone forever though! My only fear is that we'd

end up with limited set of supply and gnd symbols that look bizzare (ala

CADSoft) and can never be changed!

Bob

On 9/3/2010 6:18 PM, Bob Starr wrote:

>>

>> So, what is the difference between using something like a supply +5V from

>> the library vs. just drawing a net and naming it +5V and giving it an xref

>> ?

>>

>> Thanks,

>>

>

You can't give supply nets arbitrary names with supply symbols as

implemented as a library component without overwriting the resulting power

net name. When you drop a power symbol on a sheet and connect it to a net,

it uses the name assigned to the SYMBOL PIN in the library SYMBOL (not the

device name) as the new power net name to assign in the schematic.

>

I can't tell you how many drawings folks have sent me with screwed up power

symbols, nets, etc due to this. For instance, if you overwrite a supply

symbol net name and then use the COPYcommand to duplicate that power symbol

and connect it to a new net, the new net will have the original name that

was assigned to the pin in the SYMBOL rather than the net it was currently

assigned to. I see lots of drawings where beginners do this and have power

nets all goofed up and/or not connected properly. I've seen lots of

improperly created power symbols with the pin name different from the

symbol/device name which can really cause havoc in a drawing with power nets

all tied incorrectly to each other.

>

In other systems, like Altium, the power symbol is a native object in the

schematic and you can give it any arbitrary name you like when you add a

power symbol. Your limited to a few power symbol types (like a t-bar, circle

or arrow), but I like this for consistency reasons. If you duplicate the

symbol and connect it to another net, then  it uses the arbitrary name

assigned to that symbol instance (rather than using the original name from a

lib object). None of this business of  "the power symbol net name was

overwritten" warnings or confusion exists.

>

It wouldn't be that big of a deal to add a native power symbol object in the

schematic editor. But, converting all the old drawings that use the lib

power symbols would be a little bit of a conversion headache.  I'd be

perfectly happy to see these gone forever though! My only fear is that we'd

end up with limited set of supply and gnd symbols that look bizzare (ala

CADSoft) and can never be changed!

>

Bob

>

>

I also dislike the "predefined net" behavior of the power symbols.

I have considered making some "dummy" power symbols that act like the

"named ports" in the dports library and just using EAGLE's normal net

naming/connecting facility. But it would be nice if it automagically

popped up the name of the net without having to name it and label it,

and then could be COPYed to spread it around the schematic. As you said,

it would be good if this ability were built in and we could draw

whatever symbol we liked. Maybe a pin visibility called "Net Name" that

caused the displayed pin label to inherit the net name it's connected to

or something like that. who knows. maybe someone has a better idea...

maybe a ULP could encapsulate all these functions and add a new class of

power symbols like in Altium.

If something like this could be made, I would just leave the other

system intact for those who still want to use it or for compatibility,

no need to convert headache.

Hi,

While the xrefs do work, I think they look terrible on the schematic.  It may seem like a lot of work, but I'm just going to create a library item for each type that I want.  It is the difference between this:

[img]http://home.earthlink.net/~alank2/avr/nettype.gif[/img]

http://home.earthlink.net/~alank2/avr/nettype.gif

PD6 is an xref

and

PD5 is a library component using the SUP type named PD5.

Is there a way to adjust the xref size?  If I could make it smaller I'd probably just use xref's.

Thanks,

Alan