Is there anything wrong with placing vias on surface mount pads?

[Mike Noone]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

-Mike

 

[Terry Given]

For hand soldering it might work okay, but it tends to wick the solder
down the via, causing a dry joint or tomb stoning (the part is pulled up
on one end during re flow soldering by the uneven surface tension).

unless you use a very, very small hole ($$$)

Cheers
Terry

 

[John Popelish]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

For hand soldering it might work okay, but it tends to wick the solder
down the via, causing a dry joint or tomb stoning (the part is pulled
up on one end during re flow soldering by the uneven surface tension).

 

[Hal Murray]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

google for via-in-pad.

It's sometimes used to reduce the inductance on bypass caps.

The usual problem is that the hole in the via sucks up some
of the solder applied by the normal solder-paste through a
stencil approach so there isn't enough left for a good solder
joint. That shouldn't be a problem if you are hand soldering
a proto board.

Make sure you have enough room to get the soldering iron in
to solder the resistors.

 

[Robert Baer]

unless you use a very, very small hole ($$$)

Cheers
Terry

Better yet, use same size hole on both pads, and centered.

 

[Terry Given]

Better yet, use same size hole on both pads, and centered.

unless its a big hole - reductio ad absurdum, it better be smaller than
the pad.....

some contract manufacturers may refuse to make such a PCB.

Cheers
Terry

 

[Fred Bartoli]

unless its a big hole - reductio ad absurdum, it better be smaller than
the pad.....

some contract manufacturers may refuse to make such a PCB.

Making the PCB? Why would they?

Of course, making the whole assembly is another matter.

 

[Joerg]

Hello Mike,

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

I wouldn't do that. With one exception: When I need a really low
impedance to other layers, for example in case of a connection area for
chassis ground or a high amperage power supply cable (the garden hose
size wires).

Consider smaller resistors. You can go much smaller than 0603 and
nowdays smaller sizes are almost standard. But mind the dissipation,
probably need to run ye olde HP calculator on every resistor that is low
enough in ohms and across a few volts.

Regards, Joerg

 

[Terry Given]

Making the PCB? Why would they?

Of course, making the whole assembly is another matter.

dont laugh, i really have had contract mfgs piss and moan about IPCD275
and IPCSM782 - no comply, no build. And I meant populate the pcb, not
fabricate it (although I have had a pcb mfg refuse to make single-sided
PCBs with rivets, cant say as I blame them).

Cheers
Terry

 

[Boris Mohar]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

-Mike

If you are hand soldering the you can get away with it. Otherwise use
conductive via plug CB100 from Dupont.



Regards,

Boris Mohar

Got Knock? - see:
Viatrack Printed Circuit Designs (among other things) http://www.viatrack.ca

void _-void-_ in the obvious place

 

[Gary Pace]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going
to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled.
Gut
instinct says go for it, but my layout editor is yelling at me so I
thought
I should check just to be sure. Thanks,

-Mike

I think some fab manufacturers can solid-fill (plug) the via so the solder
doesn't wick down the hole.

 

[Al]

I think some fab manufacturers can solid-fill (plug) the via so the solder
doesn't wick down the hole.

The problem with vias on pads that are soldered is that they develop
circumferential fractures at the via/pad joint. Now if the via is solder
filled, then the fracture may not bother you. If you hand solder them,
it really makes them problamatic.

Al

 

[Roy L. Fuchs]

If you are hand soldering the you can get away with it. Otherwise use
conductive via plug CB100 from Dupont.



Regards,

Boris Mohar

Got Knock? - see:
Viatrack Printed Circuit Designs (among other things) http://www.viatrack.ca

void _-void-_ in the obvious place

All one needs to do is MASK over the via on the other side of the
board.

 

[Roy L. Fuchs]

I think some fab manufacturers can solid-fill (plug) the via so the solder
doesn't wick down the hole.

Solder mask is silk screened on wet. All he needs to do is make
sure the mask covers any vias that he wants to keep wick free.

They only need to plug one side. It will not affect the via
integrity.

 

[John_H]

Hi - I'm working on a really, really tight layout right now. I have a
number of 0603 resistors very closely packed with a number of vias going to
them. Would it be OK to place the vias directly in the center of one of a
0603's pads? This is for a prototype board, and will be hand assembled. Gut
instinct says go for it, but my layout editor is yelling at me so I thought
I should check just to be sure. Thanks,

-Mike

"Filled vias" is what to google on. The hole-in-pad is doable but not
all PC board vendors happily provide them and it is an additional cost.