Problem connecting Power Pads to GND polygon

On 10/11/2009 10:49 PM, Graham wrote:

I am designing a board that includes several kinds of ICs

with "Power Pads" under the IC package that need

to be grounded. For some of the ICs, the GND polygon

connects to the Power Pad as it should. For other

ICs, the GND polygon is not connecting to the Power Pad.

Examining the devices in the library, they appear to be

constructed and labeled the same way. I can't see

a difference in labeling, pin declaration, or grounding

between the ones that connect to ground and the ones

that don't.

 

Can you suggest what might be different between the

ICs or the libraries to cause this?

 

Thank you,

--- Graham

 

==

My first thought is, do the gnd pads of the package have air-wires in

the PCB editor? If so, check the Isolate property for the polygon to get

them to connect.

If there are no air-wires, I'd suggest checking the Direction and Name

properties of the symbol's pin. Make sure Direction = Pwr, and that Name

= GND. That usually does it for me...

Travis

Travis:

Thank you, you put me on the trail to understanding

the problem. All parts are built with PowerPad Direction

PWR, connected to Pin named PAD, and that Pin is grounded

in the schematic.

An example of a package that will not automatically connect

is a QFN-48, Texas Instruments footprint RGZ, for TLV320AIC33.

In this case, the edge of the power pad is within 18 mils of

peripheral SMTs, and with isolate set to 8 mils, there is

just not enough room for the polygon to get in between

the edge SMTs and the PowerPad, so no connection is made, even

though all are named GND.

The Polygon apparently needs more than double the isolate

number to get in between the edge and center pads.  Or perhaps

there is another setting somewhere I need to adjust.

The only way I have found to get the PowerPad to connect to

the peripheral ground SMTs is to turn off thermals for the

PowerPad.

If, as an exercise, I make the PowerPad smaller, the polygon will

connect to the PowerPad, so it is not the construction of

the part in the library as I first suspected.

This is an example of the tuning necessary for Eagle, where

the Isolate hierarchy, the Wire width of the Polygon, some

unexplained rules as to how Polygons work all interact, that

is not clearly explained anywhere that I have found.

Thank you,

--- Graham

==

Travis G wrote:

On 10/11/2009 10:49 PM, Graham wrote:

I am designing a board that includes several kinds of ICs

with "Power Pads" under the IC package that need

to be grounded. For some of the ICs, the GND polygon

connects to the Power Pad as it should. For other

ICs, the GND polygon is not connecting to the Power Pad.

Examining the devices in the library, they appear to be

constructed and labeled the same way. I can't see

a difference in labeling, pin declaration, or grounding

between the ones that connect to ground and the ones

that don't.

 

Can you suggest what might be different between the

ICs or the libraries to cause this?

 

Thank you,

--- Graham

 

==

My first thought is, do the gnd pads of the package have air-wires in

the PCB editor? If so, check the Isolate property for the polygon to get

them to connect.

 

If there are no air-wires, I'd suggest checking the Direction and Name

properties of the symbol's pin. Make sure Direction = Pwr, and that Name

= GND. That usually does it for me...

 

Travis

Is the polygon width set to a low number, like zero, to help it get into

the spaces?

also, maybe it should just be connected with a via( or as many vias as

will fit in the pad) rather than trying to get in between the pads, it

sounds like a thermal connection that needs a lot of copper to work

properly.

Hi Gary:

Eagle Help warns of setting the polygon width to a very low number,

they indicate it should be set to about the width of the

smallest feature or trace, because the solid fills are actually

a raster scan at the polygon width, and the number of scans and

the associated Gerber file get extremely large for very small widths.

A few experiments with this parameter indicate that it is not the

problem.  Setting it very low does not cure the problem.

It is really not a thermal problem in this case, as much as

enabling a very low impedance RF ground.  There will also be

vias in the power pad, but I want the lowest possible impedance

ground, and that would be helped by connecting the ground pins

to the well grounded very nearby power pad.

Thank you for your thoughts and interest.

--- Graham

==

Gary Gofstein wrote:

Is the polygon width set to a low number, like zero, to help it get into

the spaces?

 

also, maybe it should just be connected with a via( or as many vias as

will fit in the pad) rather than trying to get in between the pads, it

sounds like a thermal connection that needs a lot of copper to work

properly.

well, i haven't seen your layout, but I will guess that any trace that

will fit between your SMD's will have too much inductance at RF to be

any use, may even form resonators with the ground plane if you're really

at high freq/speed. i would say the main advantage is that they might

help isolate one SMD from another crosstalkwise. To get a low impedance

connection, i would just load the pad with vias to ground, but that's

just my feeling, haven't tested it ever. Best to copy whatever reference

layout is shown with the part, a lot of times they are on a separate app

note or white paper. good luck!

Gary:

The issue is not weaving grounds between the SMDs, but

rather getting the SMDs that are named as GND to automatically

connect to the PowerPad that is named GND and is only 0.5 mm away,

with nothing in between or nearby, other than the other SMDs for

adjacent package leads. And yes, I will have vias to inner layer GND

in the PowerPad.  All Isolate settings at 8 mil, or 0.2 mm.

This is a very fine pitch part.  0.5 mm pitch on the leads.

So SMDs 0.28 mm wide, and on 0.5 mm centers.  The PowerPad comes

within 0.5 mm of the SMDs for the leads.  I am having the same problem

with a QFN-16 package with a relatively large PowerPad.  Smaller

PowerPads do not have the problem.

If the PowerPad is smaller in size, and is perhaps shrunk so that

it is 1.5 mm away, the Ground Polygon will connect the SMDs named

GND to the PowerPad named GND.  If it is much closer, set to the

0.5 mm specified in the Texas Instruments footprint, the Polygon

will not connect without turning off "Thermals" on the PowerPad.

That is OK as a workaround, but I find the behavior confusing.

Software is 5.6.0 Professional on Windows XP.

--- Graham

==

Gary Gofstein wrote:

well, i haven't seen your layout, but I will guess that any trace that

will fit between your SMD's will have too much inductance at RF to be

any use, may even form resonators with the ground plane if you're really

at high freq/speed. i would say the main advantage is that they might

help isolate one SMD from another crosstalkwise. To get a low impedance

connection, i would just load the pad with vias to ground, but that's

just my feeling, haven't tested it ever. Best to copy whatever reference

layout is shown with the part, a lot of times they are on a separate app

note or white paper. good luck!

now i understand your problem. my stupidity, you clearly wrote your

title to be "connecting". now it all makes sense.

so your pad is so big that you can't form a proper thermal for the SMD,

hence EAGLE substitutes no connection! the only things i can think of,

you've already done, turn off thermals or add connections by hand. i'd

turn off the thermals or maybe you could adjust their size? i'd just

turn them off as you've done.