Searching \ for '[EE] Eagle ERC questions' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=eagle
Search entire site for: 'Eagle ERC questions'.

Exact match. Not showing close matches.
PICList Thread
'[EE] Eagle ERC questions'
2008\07\20@145516 by Kevin

picon face
Hi,

Been a while since I posted. Anyway, I am designing a board
in Eagle, and when I do an ERC check on the schematic I get
this error.

SUPPLY pin GND overwritten with more than one signal(H-GND,
GND)

I changed the net class for those pins to be H-GND for a
heavier trace width. I am not sure where it's getting the
GND signal from ?

I tried the archives and google, etc... but no luck. I basically
 have the GND pins on the M33887
chip tied to a GND symbol and then changed the net class to
H-GND so that it  has the track width set at 60 mils with 15
mils of clearence.

Thanks,
Kevin

2008\07\20@203955 by Bob Blick

face
flavicon
face
Hi Kevin,

I'm relabeling this [EE] since it fits better there and you'll get a
wider audience.

Kevin wrote:
{Quote hidden}

2008\07\20@215955 by kben

picon face
Thanks Bob.

I basically have five net classes in Eagle v5.1
signal,gnd20,gnd40,pwr20, and pwr40.
The gnd20 goes to the logic chips, and the gnd40 goes to the
motor control chip.
If I use the INFO command I can change NET CLASS, but not the NET NAME.
It says to use the NAME command to change the name.
If I use the NAME command it won't let me use the NET NAME I want it says
already in use and tries to connect the NET class with the old name.

I just wanted to run heavier tracks (40mil) for the 12V motor chip and 20
mil for the logic chips.

Can I do this in Eagle ?  I tried an old v4.15 but, it says I need at
least v4.60 to open the schematic.

Thanks,
Kevin

{Quote hidden}

> -

2008\07\21@010726 by William \Chops\ Westfield

face picon face

On Jul 20, 2008, at 6:59 PM, spam_OUTkbenTakeThisOuTspamdca.net wrote:

> Can I do this in Eagle ?  I tried an old v4.15 but, it says I need at
> least v4.60 to open the schematic.

The short answer is "no."  It is a FAQ and an often-requested feature  
to allow one signal name to have multiple classes (especially analog  
vs digital gnd, and Power vs the short traces to fine-pitch SMT  
pins), but the "one class per signal" bit seems to be very entrenched  
in the design, so it hasn't changed in a long time and doesn't look  
like it's likely that it WILL change in the foreseeable future.

The usual fixes involve various sorts of zero-ohm resistors used to  
connect the nets with the same potential but different names, or  
separate routing steps before and after changing the class  
definition, or manual routing, or living with lots of design rule  
warnings (one thing that IS possible in v5.x is to tell eagle to  
ignore certain warnings.)

BillW

2008\07\21@032728 by Xiaofan Chen

face picon face
On Mon, Jul 21, 2008 at 1:07 PM, William Chops Westfield <.....westfwKILLspamspam@spam@mac.com> wrote:
>
> On Jul 20, 2008, at 6:59 PM, kbenspamKILLspamdca.net wrote:
>
>> Can I do this in Eagle ?  I tried an old v4.15 but, it says I need at
>> least v4.60 to open the schematic.
>
> The short answer is "no."  It is a FAQ and an often-requested feature
> to allow one signal name to have multiple classes (especially analog
> vs digital gnd, and Power vs the short traces to fine-pitch SMT
> pins), but the "one class per signal" bit seems to be very entrenched
> in the design, so it hasn't changed in a long time and doesn't look
> like it's likely that it WILL change in the foreseeable future.

Hmm, do you know any EDA package to allow one net name to
have multiple Net Class associations? As far as I know, Altium P-CAD
does not allow that. Mentor Graphics Expedition Design Capature
does not allow that either.

> The usual fixes involve various sorts of zero-ohm resistors used to
> connect the nets with the same potential but different names, or
> separate routing steps before and after changing the class
> definition,

Last time we tried this with P-CAD and it did not work too well.

> or manual routing,

I believe this is the way to go.

>or living with lots of design rule
> warnings (one thing that IS possible in v5.x is to tell eagle to
> ignore certain warnings.)

We still use the design rules to check the creepage/clearance
between different Net Class. However, manual check is also
necessary. Sometimes we need to get the help from
Mechanical Engineers (inside Pro-Engineer) to check 3-D
distance.

Xiaofan

2008\07\21@074114 by Kevin
picon face
I'll look for the FAQ, I read the tutorials and did not see
an answer to my questions. But, maybe I am dense I don't want
one signal with multiple classes. I have two classes and two
signal names. I.E. I want all A-GND signals to use the GND40
(40mil) class and all D-GND signals to uses the GND20
(20mil) class. Surely this is possible ?

Regards,
Kevin

{Quote hidden}

--
Kevin

2008\07\21@080042 by olin piclist

face picon face
> SUPPLY pin GND overwritten with more than one signal(H-GND,
> GND)

Eagle thinks the name of the net connected to a supply pin should be the
same as the name of the supply pin.  I think that's a silly rule and makes
the ERC less useful, but there is no way to shut it off that I know of.  You
just have to go thru all ERC warnings and make sure none of them are "real".


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000.

2008\07\21@081604 by olin piclist

face picon face
kben@dca.net wrote:
> I basically have five net classes in Eagle v5.1
> signal,gnd20,gnd40,pwr20, and pwr40.
> The gnd20 goes to the logic chips, and the gnd40 goes to the
> motor control chip.

You are confusing net classes with the net name.  Each net can only have one
class and one name.  You can't assign one class to a part of a net and
another to the rest.

I usually use one of two solutions.  The first is to manually route critical
parts of nets.  You probably want to do this anyway if you need large
current capability since you don't want those tracks going all over the
place and you want to keep the current loops to a minimum and you have to
carefully think about ground offset voltages.  You can manually route with
any width and drill size regardless of the net class.  I usually manually
route all ground connections because I usually have a ground plane or pseudo
ground plane.  In those cases, I want each ground SMD pad with its own via
straight to the ground plane.  This is usually better for the signals and
makes subsequent routing easier.

The second method is to break up a logical net into multiple Eagle nets by
using "short" devices.  These are just copper with two connections.  I draw
them as a slightly thickened line on shematics.  To Eagle each side of the
short will be a different net.  This technique is particularly useful to
guarantee that the ground connection for some part of the circuit connects
at exactly one point that you can place to the rest of the circuit.  This
allows you, for example, to keep switching power supply loop currents
isolated and off the main ground plane.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000.

2008\07\21@083344 by olin piclist

face picon face
Kevin wrote:
> I have two classes and two signal names.

But I thought you were trying to apply them to one net.  Each net can have
only one name and one class.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000.

2008\07\21@093558 by Kevin

picon face
No, I have two nets, and two classes, with different signal
names.  It must be a bug in v5.1, or a prodedural error. I
was able to delete all my Digital Grounds and then change
the net and class to what I wanted.

Analog  GND, Net Name "A-GND", Net Class "GND40"
Digital GND, Net Name "D-GND", Net Class "GND20"

Regards,
Kevin


> Kevin wrote:
>> I have two classes and two signal names.
>
> But I thought you were trying to apply them to one net.  Each net can have
> only one name and one class.
>

More... (looser matching)
- Last day of these posts
- In 2008 , 2009 only
- Today
- New search...