Newbee: howto make device with 2 GND pins

"Rens" <rens.kessener@onsbrabantnet.nl> wrote in message

news:hr22dk$oue$1@cheetah.cadsoft.de...

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting  one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

 

 

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the

CadSoft EAGLE community meets.

 

in the symbol, name one pin GND, and the other GND@1

"Rens" <rens.kessener@onsbrabantnet.nl> wrote in message

news:hr22dk$oue$1@cheetah.cadsoft.de...

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting  one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

    I was in a hurry with previous answer.

I now see your problem: You defined the pads in the right way, but you are

bothered by the fact that Eagle wants you to connect those 2 pads with a

wire on board.

    From all I know, it's not possible to have 2 pins on the same signal,

and tell Eagle that those pins are connected together IN the IC. So just

ignore that airwire. (This is the way I would do.)

Am 25.04.2010 20:41, schrieb Rens:

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

 

 

Eagle does not know internal connections. So the rule is one pin for one

pad. Some SO8 transistors have four drains which are internally

connected. They are named D, D@1, d@2, D@3 in the library in this

example. It would be ok, if you connect just one of these pins in the

schematic and eagle would do the same in board.

BUT, why should a manufactorer add more pads, if one is enough?

Because the chip is connected to the pads with bonding wires and one

wire is not thick enough to carry the amount of current specified in the

data sheet. So two or more connections are used in parallel to carry the

current. So you should see that all equal named pins are connected

externally to avoid a "slow blowing fuse" device.

--

Gruß / regards

Joern

Thanks, That helps. Took me 2 days of reading and trying.

Advantage is that while doing that I learned many other things as a newbee.

Thanks again. Rens

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Thanks, but I figured that out already.

My problem was (with a TLE4242) that I had to cross another wire

to solve the airwire by a connection from pin 4 (GND) to the Thermal Pad

(also GND).Ignoring the airwire is the best option I understood.

Regards, Rens

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Joern Paschedag wrote:

Am 25.04.2010 20:41, schrieb Rens:

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

 

 

 

Eagle does not know internal connections. So the rule is one pin for one

pad. Some SO8 transistors have four drains which are internally

connected. They are named D, D@1, d@2, D@3 in the library in this

example. It would be ok, if you connect just one of these pins in the

schematic and eagle would do the same in board.

BUT, why should a manufactorer add more pads, if one is enough?

Because the chip is connected to the pads with bonding wires and one

wire is not thick enough to carry the amount of current specified in the

data sheet. So two or more connections are used in parallel to carry the

current. So you should see that all equal named pins are connected

externally to avoid a "slow blowing fuse" device.

 

What is the significance (if any) of using the "@" symbol in the example

  above.

BTW, what I do in this situation is have GND1, GND2, GND3, .... as pin

names on the symbol and then connect them all independently to "GND" on

the schematic.  Works well.

On 4/26/2010 2:13 PM, Michael Sansom wrote:

Joern Paschedag wrote:

Am 25.04.2010 20:41, schrieb Rens:

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

 

 

 

Eagle does not know internal connections. So the rule is one pin for

one pad. Some SO8 transistors have four drains which are internally

connected. They are named D, D@1, d@2, D@3 in the library in this

example. It would be ok, if you connect just one of these pins in the

schematic and eagle would do the same in board.

BUT, why should a manufactorer add more pads, if one is enough?

Because the chip is connected to the pads with bonding wires and one

wire is not thick enough to carry the amount of current specified in

the data sheet. So two or more connections are used in parallel to

carry the current. So you should see that all equal named pins are

connected externally to avoid a "slow blowing fuse" device.

 

 

What is the significance (if any) of using the "@" symbol in the example

above.

 

BTW, what I do in this situation is have GND1, GND2, GND3, .... as pin

names on the symbol and then connect them all independently to "GND" on

the schematic. Works well.

 

The part following the '@' is not shown so that each looks like the same

label pin.

On Mon, 26 Apr 2010, Michael Sansom wrote to us saying :

What is the significance (if any) of using the "@" symbol in the

example  above.

 

The @ symbol in a pin name introduces a hidden suffix, so that it allows

all the pins to appear on the schematic as just "GND". It also means the

net table treats them as just "GND", so they all get automatically

connected to the GND net.

BTW, what I do in this situation is have GND1, GND2, GND3, .... as pin

names on the symbol and then connect them all independently to "GND" on

the schematic.  Works well.

Yes, that works, but it requires you to explicitly connect them all,

shows a fake ordering of ground connections, and usually doesn't match

the data sheet. It's very reasonable for the tab of a SOT223 FET, where

you may actually want to distinguish between the tab and the middle pin

because you only actually need to connect one of them, but for a 64 pin

LQFP chip with 8 ground pins, you want them all to be the same to ensure

they're all connected (like the data sheet says they must be).

--

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

The contents of this | Windows NT crashed.

message are purely   | I am the Blue Screen of Death.

my opinion. Don't    | No one hears your screams.

believe a word.      |

Am 27.04.2010 00:24, schrieb Gary Gofstein:

On 4/26/2010 2:13 PM, Michael Sansom wrote:

Joern Paschedag wrote:

Am 25.04.2010 20:41, schrieb Rens:

Like SOT223 a device having 2 pins internally connected in the device.

Sot224 pin 2 and 4(cooling pad) are the same.

I supposed that connecting one pin it is also connected to the other.

However, on the board a airwire still remains. This is also true for a

sot223 device from the library.

I tried the mailto:GND@1 etc. naming, but seems not to work.

What am I doing wrong?

 

 

 

Eagle does not know internal connections. So the rule is one pin for

one pad. Some SO8 transistors have four drains which are internally

connected. They are named D, D@1, d@2, D@3 in the library in this

example. It would be ok, if you connect just one of these pins in the

schematic and eagle would do the same in board.

BUT, why should a manufactorer add more pads, if one is enough?

Because the chip is connected to the pads with bonding wires and one

wire is not thick enough to carry the amount of current specified in

the data sheet. So two or more connections are used in parallel to

carry the current. So you should see that all equal named pins are

connected externally to avoid a "slow blowing fuse" device.

 

 

What is the significance (if any) of using the "@" symbol in the example

above.

 

BTW, what I do in this situation is have GND1, GND2, GND3, .... as pin

names on the symbol and then connect them all independently to "GND" on

the schematic. Works well.

 

The part following the '@' is not shown so that each looks like the same

label pin.

...and gnd1, gnd2 or vdd1 and vdd2 etc. are usually different nets if

you use an isolation amplifier for example

--

Gruß / regards

Joern

On 04/26/2010 04:22 AM, Joern Paschedag wrote:

...

BUT, why should a manufactorer add more pads, if one is enough?

Because the chip is connected to the pads with bonding wires and one

wire is not thick enough to carry the amount of current specified in the

data sheet. So two or more connections are used in parallel to carry the

current. So you should see that all equal named pins are connected

externally to avoid a "slow blowing fuse" device.

Don't forget thermal considerations.  Each pin will carry some heat away

from the die.  So connecting these externally is essential if you expect

to meet the theta-ja specs.

Enjoy,

    - Chuck