Standard for size of plated through holes?

F

fellow

Guest
What Standard defines the size of plated through holes in a PCB?
Thanks
 
In article <ctmgi1$ei1$1@news7.svr.pol.co.uk>, Jameson@god.com says...
What Standard defines the size of plated through holes in a PCB?
Thanks



Any size hole in a PCB can be plated through. The PCB house will
Click to expand...
generally drill the hole a few mils larger than you specify so that
the plating will reduce the hole size to near that which you
specified.

Plating through very small holes (smaller than 0.019") can require
special processing and may raise the board cost or limit your
choice of vendors.

Mark Borgerson
 
You need to talk to your board house about minimum plated hole sizes.
We commonly use 0.010" dia via sizes, sometimes down to 0.008" dia.

If you're thinking about hole size for through-hole component leads,
the one of the IPC standards may have the proper info.
http://webvision.ipc.org/scripts/mgrqispi.dll?APPNAME=IPCWEB&PRGNAME=TOCFRAME&ARGUMENTS=-N,-N,-A,-A,-N50
 
"fellow" <Jameson@god.com> wrote in message
news:ctmgi1$ei1$1@news7.svr.pol.co.uk...
What Standard defines the size of plated through holes in a PCB?
Click to expand...
Depends on the board supplier. I use PCB-Pool a lot for prototypes and their
minimum size is 0.3 mm for double-sided and four-layer boards.

Leon
 
"qrk" <spamtrap@reson.com> wrote in message
news:1107231339.654978.171040@z14g2000cwz.googlegroups.com...
You need to talk to your board house about minimum plated hole sizes.
We commonly use 0.010" dia via sizes, sometimes down to 0.008" dia.

If you're thinking about hole size for through-hole component leads,
the one of the IPC standards may have the proper info.

http://webvision.ipc.org/scripts/mgrqispi.dll?APPNAME=IPCWEB&PRGNAME=TOCFRAME&ARGUMENTS=-N,-N,-A,-A,-N50

Thanks. But dunno which one. I should have made it clear that I'm interested
Click to expand...
in plated through holes for components, so obviously they must be a minimum
size for the purposes of solderability
 
fellow wrote:

Thanks. But dunno which one. I should have made it clear that I'm interested
in plated through holes for components, so obviously they must be a minimum
size for the purposes of solderability
Click to expand...
From a practical point of view, anything from 25% to 50% larger than the component
lead will solder nicely. If you go much smaller, you will rip out the plated holes
when you try to rework the board. Much larger, and you will have trouble filling the
holes with solder.

-Chuck
 
ANSI/IPC-2222, "Sectional Design Standard for Rigid Organic Printed
Boards"
Table 9-3
 
On Wed, 2 Feb 2005 02:01:11 -0000, "fellow" <Jameson@god.com> wrote:


Thanks. But dunno which one. I should have made it clear that I'm interested
in plated through holes for components, so obviously they must be a minimum
size for the purposes of solderability
Click to expand...
I use .035" for most component leads - ICs, 1/4W resistors, etc. The
..025" square post headers need .040.

Holes should normally be about .010 or so larger than the component
lead.

I use .025" for via holes - at one point the board shop charged extra
for .024 or less, so that set my via size.



--
Peter Bennett VE7CEI
email: peterbb4 (at) interchange.ubc.ca
GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html
Newsgroup new user info: http://vancouver-webpages.com/nnq
 
"fellow" <Jameson@god.com> wrote in message
news:ctpai0$kc3$1@news7.svr.pol.co.uk...
"qrk" <spamtrap@reson.com> wrote in message
news:1107231339.654978.171040@z14g2000cwz.googlegroups.com...
You need to talk to your board house about minimum plated hole sizes.
We commonly use 0.010" dia via sizes, sometimes down to 0.008" dia.
If you're thinking about hole size for through-hole component leads,
the one of the IPC standards may have the proper info.


http://webvision.ipc.org/scripts/mgrqispi.dll?APPNAME=IPCWEB&PRGNAME=TOCFRAME&ARGUMENTS=-N,-N,-A,-A,-N50
Click to expand...


Thanks. But dunno which one. I should have made it clear that I'm
interested
in plated through holes for components, so obviously they must be a
minimum
size for the purposes of solderability
Click to expand...
Consider a PCB in front of you, like a old motherboard with a intel 286.
Desolder an IC without damage. The hole size will be about 0.030"
+/- 0.005 ? The IC pins will be about 0.020". Take a brand new DIP
IC and measure the pins with some calipers. Add 0.010" to the pin
size. That's you drill hole size. That's your standard.

As to any standard? I havn't bothered to look around. The last standard
I used was IPC-610. It's all changed now.

Find out who sells PCB drills. Look at the Drills sizes being used by the
CNC machine.

http://www.uniontool.co.jp/english/tech_05.html

http://www.kyoceratycom.com/products/pcb_drills.htm

http://www.thinktink.com/stack/volumes/volvi/drilling.htm
http://www.thinktink.com/stack/volumes/voli/store/drillsup.htm

http://northbaytechnical.com/standard1.htm

http://cutting-tools.globalspec.com/LearnMore/Manufacturing_Process_Equipment/Cutting_Tools/Drill_Bits

etc,

What I learned is make all the holes on the PCB 0.030 or 0.040"
Why? Because, imagine if you will. You layout your board and use
the defaults from the CAD your using. Unknowingly, the drill file
makes 10 different drill size call outs. The Gerber drill files will tell
you
at a glance, what's with all these Gerber drill files?

Imagine, a guy standing infront of a CNC drilling machine.
You called out for a 0.008" drill hole. The guy has probably 100's of
different drills sizes, in thousandths of an inch and millimeter sizes.
The drill guy has to find a drill that small. If he dosen't have it, then
he
has to order it... It Takes Time. Your time in the end.

Also small drill bits break. What happens if the drill breaks while
drilling out your board, or someone elses board? Production stops
till the drill gets changed out. Damage acessment by the Board House
QC as to damage accessment to your stack of boards he's drilled out
so far. Now... do we have to cut more blank boards because the drill
broke in the middle of the board stack, the booklet? Yes or No?
etc. What's a booklet? Your PCBs start by cutting 3 blank copper
boards, stacking them together, pinning them together so they don't
move during the drilling process. These 3 blank boards are a booklet.

Drill guy has to change the drill bits, because you called out for so many
different holes. That means stopping the CNC drill machine, changing
the drill bit, load the new Gerber drill file and start drilling. It Takes
Time.
And then what happens if another drill bit breaks in the middle a job?
Well, you have to start all over from scratch. Happens all the time,
all day long.

Question, what will you gain if the via is 0.030" or 0.008" ?
I've never seen a difference. Once the board is soldered, who cares?
The wave solder will fill in all the holes. If mfg. is by hand, so you have
non soldered vias, so what. If you can replace 5 drill hole sizes with a
0.015" drill size, that would be good. If you could replace all drill sizes
with 0.030" that would be great. Imagine again the CNC machine, the
guy who has to chuck the drill bit, load the CNC file for that Gerber
drill size, stop the CNC machine every time to chuck the next drill size,
do this tillyou board is done. What happens if all the holes are one
size? The drill guy sets up that one drill bit size and the board is done.
The drilled out board goes to QC for inspection under a microscope
and measure a few hole locations, to match up with the artwork.
Tell me you havn't seen a board where the holes were off a bit, the trace
makes it to the DIP part or via, but it's off a bit, board ohms out ok,
ship it.

1. Design a PCB.
2. Create as fewer Gerber files as possible
3. Send to boards house as a few a Gerber files as possible.
4. Get PCBs made faster.

cya
Ed
 
Ed,
did you have to write a book to explain what could have been
said in one paragraph? Besides which your details are pretty
sketchy. You sound kind of like the guy that stayed at a Holiday
Inn Express last night.
Volume does not equal quality. In your case a lot less volume
would have been more accurate and correct.

(i.e. IPC-610C is an acceptability standard and has nothing
whatsoever to do with specifying holes sizes. Nobody stops the
CNC machine to change each bit size. There is a tool caddy that
typically holds a minimum of 8 tools/bits. Greater than eight
tools they will partition the file so that there is one pause to
enter the next set of up to 8 drill sizes required. It takes
seconds to change the bits in the caddy for the second partition.
Smaller via sizes gain you routing area, larger vias require
larger pads and take more area. But, larger vias can carry more
current and plate through better. You use as many Gerber files as
necessary for the layer detail of the board (note: nothing to do
with drills), no more, no less. The drills are not dealt with via
a Gerber file but rather an Excellon or Ascii format drill file.)

--
Sincerely,
Brad Velander

"EN" <res808c4@earthlink.net> wrote in message
news:%M15e.4754$44.563@newsread1.news.atl.earthlink.net...
"fellow" <Jameson@god.com> wrote in message
news:ctpai0$kc3$1@news7.svr.pol.co.uk...

"qrk" <spamtrap@reson.com> wrote in message
news:1107231339.654978.171040@z14g2000cwz.googlegroups.com...
You need to talk to your board house about minimum plated
hole sizes.
We commonly use 0.010" dia via sizes, sometimes down to
0.008" dia.
If you're thinking about hole size for through-hole
component leads,
the one of the IPC standards may have the proper info.



http://webvision.ipc.org/scripts/mgrqispi.dll?APPNAME=IPCWEB&PRGNAME=TOCFRAME&ARGUMENTS=-N,-N,-A,-A,-N50


Thanks. But dunno which one. I should have made it clear that
I'm
interested
in plated through holes for components, so obviously they
must be a
minimum
size for the purposes of solderability

Consider a PCB in front of you, like a old motherboard with a
intel 286.
Desolder an IC without damage. The hole size will be about
0.030"
+/- 0.005 ? The IC pins will be about 0.020". Take a brand
new DIP
IC and measure the pins with some calipers. Add 0.010" to the
pin
size. That's you drill hole size. That's your standard.

As to any standard? I havn't bothered to look around. The last
standard
I used was IPC-610. It's all changed now.

Find out who sells PCB drills. Look at the Drills sizes being
used by the
CNC machine.

http://www.uniontool.co.jp/english/tech_05.html

http://www.kyoceratycom.com/products/pcb_drills.htm

http://www.thinktink.com/stack/volumes/volvi/drilling.htm
http://www.thinktink.com/stack/volumes/voli/store/drillsup.htm

http://northbaytechnical.com/standard1.htm


http://cutting-tools.globalspec.com/LearnMore/Manufacturing_Process_Equipment/Cutting_Tools/Drill_Bits

etc,

What I learned is make all the holes on the PCB 0.030 or 0.040"
Why? Because, imagine if you will. You layout your board and
use
the defaults from the CAD your using. Unknowingly, the drill
file
makes 10 different drill size call outs. The Gerber drill
files will tell
you
at a glance, what's with all these Gerber drill files?

Imagine, a guy standing infront of a CNC drilling machine.
You called out for a 0.008" drill hole. The guy has probably
100's of
different drills sizes, in thousandths of an inch and
millimeter sizes.
The drill guy has to find a drill that small. If he dosen't
have it, then
he
has to order it... It Takes Time. Your time in the end.

Also small drill bits break. What happens if the drill breaks
while
drilling out your board, or someone elses board? Production
stops
till the drill gets changed out. Damage acessment by the Board
House
QC as to damage accessment to your stack of boards he's drilled
out
so far. Now... do we have to cut more blank boards because
the drill
broke in the middle of the board stack, the booklet? Yes or
No?
etc. What's a booklet? Your PCBs start by cutting 3 blank
copper
boards, stacking them together, pinning them together so they
don't
move during the drilling process. These 3 blank boards are a
booklet.

Drill guy has to change the drill bits, because you called out
for so many
different holes. That means stopping the CNC drill machine,
changing
the drill bit, load the new Gerber drill file and start
drilling. It Takes
Time.
And then what happens if another drill bit breaks in the middle
a job?
Well, you have to start all over from scratch. Happens all the
time,
all day long.

Question, what will you gain if the via is 0.030" or 0.008" ?
I've never seen a difference. Once the board is soldered, who
cares?
The wave solder will fill in all the holes. If mfg. is by
hand, so you have
non soldered vias, so what. If you can replace 5 drill hole
sizes with a
0.015" drill size, that would be good. If you could replace all
drill sizes
with 0.030" that would be great. Imagine again the CNC
machine, the
guy who has to chuck the drill bit, load the CNC file for that
Gerber
drill size, stop the CNC machine every time to chuck the next
drill size,
do this tillyou board is done. What happens if all the holes
are one
size? The drill guy sets up that one drill bit size and the
board is done.
The drilled out board goes to QC for inspection under a
microscope
and measure a few hole locations, to match up with the artwork.
Tell me you havn't seen a board where the holes were off a bit,
the trace
makes it to the DIP part or via, but it's off a bit, board ohms
out ok,
ship it.

1. Design a PCB.
2. Create as fewer Gerber files as possible
3. Send to boards house as a few a Gerber files as possible.
4. Get PCBs made faster.

cya
Ed
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top