Connecting multiple pins to one pad SO8 M OSFET

On 20/03/14 17:26, Kirk Sceviour wrote:

Hi;

 

Looking for some help on getting the multiple Drain and Source pads of a

N-Channel MOSFET to connect. All of these pins should be connected on the

board to allow for the 1A capability. This device is a DMS3016SSS in SO8

form factor. The device is N-MOSFET-So8S from transistor-power.lbr. I'ts

not an exact match for the chip but close enough.

 

Unfortunately it appears to be a broken library part.

The source and drain both have multiple pins along the same line, so

that they're largely hidden. The idea is that you connect to all of them

with the same net, by clicking on each one along the line in the schematic.

Unfortunately, as I said, it's broken, because in order to fit all the

pins in a small space they have NOT been placed on a 0.1" grid, which

makes it impossible to connect to all of them.

Thanks for the input. I was working on this while waiting for a reply. I

solved the problem by rewiring the symbol to show each pin individually and

wiring them appropriately in the schematic. I was beginning to think the

part part was incorrectly made. I'm now able to connect the pins the way I

want using a polygon with thermals.

Thanks for your help.

--

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

On 21/03/2014 6:26 a.m., Kirk Sceviour wrote:

Hi;

 

Looking for some help on getting the multiple Drain and Source pads of a

N-Channel MOSFET to connect. All of these pins should be connected on the

board to allow for the 1A capability. This device is a DMS3016SSS in SO8

form factor. The device is N-MOSFET-So8S from transistor-power.lbr. I'ts

not an exact match for the chip but close enough.

 

Pins 1 to 3 are Source. Pins 5 to 8 are all Drain pins.  Pin 4 is the Gate.

In the schematic the Gate pin connects properly however only only of the

Source pins connects (Pin 1) and only one of the Drain pins connect (Pin

5). They can't all be seen but the required drain and source pins are

present in the symbol (laid on top of each other). All the Drain and Source

pins have a PAS function applied. I've managed to get the Drain pins (5-8)

all on the same pad using a simple rectangle and approving the overlap

warning generated by the rule check however the Source pins won't accept

this. I've tried using a polygon named the same as the net on Pin 1 as well

as a simple rectangle to get these pins to connect on the board but it's

not working out. The Source pins will not agree to be on the same pad. The

MOSFET is being used in an unusual application and the Source pins in this

design all all connected to ground. The board has a ground polygon around

it.

 

Any suggestions?

 

When I look at that device (v6.5.0) it is perfect.

The symbol only has 3 pins and those three pins connect to the correct

(multiple) pads of the package as you describe. Perhaps you are using an

older Eagle version or an old library?

HTH

Warren

The symbol has 8 pins. The ones you can't see are underneath the visible

Drain and Source pins. Yes a MOSFET only has three pins (D/G/S) however its

in an SO8 package which has 8 pins. The extra 5 pins are internally

attached to the Drain and Source pins of the MOSFET. The transistor is

rated for 1A of current so these pins should not be left unconnected on the

board. Usually the pins are all soldered to a single pad however I couldn't

get these to connect. I ended up moving the hidden pins so they could be

seen in the schematic and wired appropriately. That way I could enclose the

pads in polygons and create large copper pours to solder the Drain and

Source pads to.

--

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

On 22/03/2014 2:11 p.m., Kirk Sceviour wrote:

The symbol has 8 pins. The ones you can't see are underneath the visible

Drain and Source pins. Yes a MOSFET only has three pins (D/G/S) however its

in an SO8 package which has 8 pins. The extra 5 pins are internally

attached to the Drain and Source pins of the MOSFET. The transistor is

rated for 1A of current so these pins should not be left unconnected on the

board. Usually the pins are all soldered to a single pad however I couldn't

get these to connect. I ended up moving the hidden pins so they could be

seen in the schematic and wired appropriately. That way I could enclose the

pads in polygons and create large copper pours to solder the Drain and

Source pads to.

 

 

I have extracted the part, I was describing in the Eagle Library, and

attached it. Display the device, click 'connect' and you will see it

only has thee pins connected to the multiple pads of the 8pin package.

Just the way it should be

Enjoy

Warren

We seem to be talking about two different packages here and unfortunately

the one you attached shows as an invalid library in my 5.11 version of

Eagle. It won't open (yes I haven't migrated yet since I have several

ongoing projects I just don't want trouble with).

If you only have 3 pins to connect in the library editor then it isn't the

same. In my version of the symbol there are 8 pins which need to be

assigned to the SO8 package to create the SO8 MOSFET device. This isn't a

problem until you place it on a board and find that there is only one Drain

and one Source pad connecting to the board, the rest are left as

unconnected pins.

I have it working now but it looks odd in the schematic because I had to

expose the extra pins on the symbol and wire them. I'm just about to remake

the symbol on .1" to see if it works correctly.

--

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

On 23/03/2014 5:28 a.m., Kirk Sceviour wrote:

We seem to be talking about two different packages here and unfortunately

the one you attached shows as an invalid library in my 5.11 version of

Eagle. It won't open (yes I haven't migrated yet since I have several

ongoing projects I just don't want trouble with).

 

If you only have 3 pins to connect in the library editor then it isn't the

same. In my version of the symbol there are 8 pins which need to be

assigned to the SO8 package to create the SO8 MOSFET device. This isn't a

problem until you place it on a board and find that there is only one Drain

and one Source pad connecting to the board, the rest are left as

unconnected pins.

 

I have it working now but it looks odd in the schematic because I had to

expose the extra pins on the symbol and wire them. I'm just about to remake

the symbol on .1" to see if it works correctly.

 

Now you have it.

Version 5 libraries are binary whereas version 6 are XML.

Eagle 6 can read v5 libraries but v5 cannot read v6 libraries.

Libraries included with each Eagle version are updated to benefit from

that version's capabilities. The library and part names stay the same as

the previous version but not backward compatible in the case of v6 to v5.

New functionality arrived in v6 that permits multiple pads per pin.

Your example, stacked pins, was the way it needed to be done prior to v6.

All the best

Warren