pcb design rules

  • Thread starter colin_toogood@yahoo.com
  • Start date
C

colin_toogood@yahoo.com

Guest
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

Any thoughts or links most appreciated.

Colin
 
On Feb 22, 11:48 am, "colin_toog...@yahoo.com"
<colin_toog...@yahoo.com> wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

Any thoughts or links most appreciated.

Colin
Click to expand...
Hi,
I depends on mostly the PCB manufacturer. If you are going to produce
mass productions ask some of the firms that you are working with I
suggest. We have different types of PCB rules for different projects
and different manufacturers. You may send your Gerber files to the
manufacturers and they usually check whether it is proper or not
before production.
Engin
 
colin_toogood@yahoo.com wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.
Click to expand...

I always make track and gap equal (unless there's an electrical reason
to do otherwise). I've found that decent PCB makers have no problem with
6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say
0.4mm or 0.5mm, if you can.

Why by the way are tracks always in thou and holes in millimetres?

Paul Burke
 
On Thu, 22 Feb 2007 16:22:33 +0000, Paul Burke <paul@scazon.com>
wrote:

colin_toogood@yahoo.com wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.


I always make track and gap equal (unless there's an electrical reason
to do otherwise). I've found that decent PCB makers have no problem with
6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say
0.4mm or 0.5mm, if you can.

Why by the way are tracks always in thou and holes in millimetres?

Paul Burke
Click to expand...
In 'merica, we use mils (thou) for drill holes.
Most decent PCB houses can deal with 5/5 mil rules. Below that, you
need to find a good house and pay more. Any wanker PCB house can
handle 10/10 rules. I routinely use 8 mil via holes for my crammed
boards. The board house will be happier if your via holes are more
like 13 to 20 mils. Before commiting to a PCB house, see if they can
show you a sample of their work. Talk to the PCB houses and find out
what rules you should follow, especially if you're trying to hit a
price target.

---
Mark
 
On 22 Feb, 16:22, Paul Burke <p...@scazon.com> wrote:
colin_toog...@yahoo.com wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

I always make track and gap equal (unless there's an electrical reason
to do otherwise). I've found that decent PCB makers have no problem with
6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say
0.4mm or 0.5mm, if you can.

Why by the way are tracks always in thou and holes in millimetres?
Click to expand...
That's quite common in the UK. I find them easy to visualise, for some
reason.

Leon
 
In article <1172176076.211930.224690@s48g2000cws.googlegroups.com>,
leon355@btinternet.com says...
On 22 Feb, 16:22, Paul Burke <p...@scazon.com> wrote:
colin_toog...@yahoo.com wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

I always make track and gap equal (unless there's an electrical reason
to do otherwise). I've found that decent PCB makers have no problem with
6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say
0.4mm or 0.5mm, if you can.

Why by the way are tracks always in thou and holes in millimetres?

That's quite common in the UK. I find them easy to visualise, for some
reason.

Leon


He stated "always" and that isn't true.
Click to expand...
We do all our design in mils, traces, holes, pads, spacings.
I think it is more of a use whatever works for you kinda' thing.

Jim
 
On 22 Feb 2007 01:48:53 -0800, "colin_toogood@yahoo.com"
<colin_toogood@yahoo.com> wrote:

Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

Any thoughts or links most appreciated.

Colin
Click to expand...
It would help to know what sort of board you are designing.

For simple boards using only through-hole components, I normally use
10 or 12 thou tracks and spaces, and 62 thou pads with 35 thou holes
for most parts. Vias are usually 50 thou pads and 25 thou holes.

Holes for component leads are usually 5 - 10 thou larger in diameter
than the leads, and pads 20 - 30 thou larger than holes (this leaves a
20 - 15 thou wide annular ring around the pad).

--
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
new newsgroup users info : http://vancouver-webpages.com/nnq
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca
 
On 23 Feb, 01:56, Peter Bennett <pete...@somewhere.invalid> wrote:
On 22 Feb 2007 01:48:53 -0800, "colin_toog...@yahoo.com"

colin_toog...@yahoo.com> wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

Any thoughts or links most appreciated.

Colin

It would help to know what sort of board you are designing.

For simple boards using only through-hole components, I normally use
10 or 12 thou tracks and spaces, and 62 thou pads with 35 thou holes
for most parts. Vias are usually 50 thou pads and 25 thou holes.

Holes for component leads are usually 5 - 10 thou larger in diameter
than the leads, and pads 20 - 30 thou larger than holes (this leaves a
20 - 15 thou wide annular ring around the pad).

--
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
new newsgroup users info :http://vancouver-webpages.com/nnq
GPS and NMEA info:http://vancouver-webpages.com/peter
Vancouver Power Squadron:http://vancouver.powersquadron.ca
Click to expand...
What I am trying to understand is for a certain track and gap what via
size I should use. Presumably the two go hand in hand so that if a
design doesn't quite fit I would be able to reduce both for the same
incremental rise in costs but all I find is "ideally use this" and
"worst case we can cope with this" but the grey area between doesn't
get a mention.

Colin
 
On Feb 23, 4:33 am, "colin_toog...@yahoo.com"
<colin_toog...@yahoo.com> wrote:
On 23 Feb, 01:56, Peter Bennett <pete...@somewhere.invalid> wrote:



On 22 Feb 2007 01:48:53 -0800, "colin_toog...@yahoo.com"

colin_toog...@yahoo.com> wrote:
Hi all

I'm trying to get a feel for what pcb design rules to use. I have
found various manufacturers sites which define their minimum track,
gap and drill size but I'm trying to work out in what order I should
be reducing each of these to get my pcb routed.

Any thoughts or links most appreciated.

Colin

It would help to know what sort of board you are designing.

For simple boards using only through-hole components, I normally use
10 or 12 thou tracks and spaces, and 62 thou pads with 35 thou holes
for most parts. Vias are usually 50 thou pads and 25 thou holes.

Holes for component leads are usually 5 - 10 thou larger in diameter
than the leads, and pads 20 - 30 thou larger than holes (this leaves a
20 - 15 thou wide annular ring around the pad).

--
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
new newsgroup users info :http://vancouver-webpages.com/nnq
GPS and NMEA info:http://vancouver-webpages.com/peter
Vancouver Power Squadron:http://vancouver.powersquadron.ca

What I am trying to understand is for a certain track and gap what via
size I should use. Presumably the two go hand in hand so that if a
design doesn't quite fit I would be able to reduce both for the same
incremental rise in costs but all I find is "ideally use this" and
"worst case we can cope with this" but the grey area between doesn't
get a mention.

Colin
Click to expand...
I use EAGLE for PCB design. All of my boards have been prototypes (2
layer and 4 layer). I typically use 10 mil (0.010") wide traces and
10 mil wide spaces. For power runs (i.e. 5v) I use 24 or 32 mil
traces. For vias, I specify a 20 mil (0.020") drill. Eagle's
standard via drill size is ~ 25 mils. To connect a heavy trace on one
side to the corresponding heavy trace on the other side, I usually use
2 20 mil vias instead of 1 large via.
HTH
-Dave Pollum
 
I'm trying to get a feel for what pcb design rules to use.
Click to expand...
Maybe this link helps.
http://www.smps.us/pcb-design.html

BTW, there is a worldwide shift to the metric system, according to IPC.
The driving force is an EC regulative.

150 micrometres width and space is common for most professional board
makers with vias as small as 0.3/0.7 mm final dimension. Minimum is 75
micrometres for larger production quantities with vias as small as
0.1/0.3 mm (bore/ring) - so called microvias. Only a few can do this.
E.g. in Germany you might find around 5 PCB manufacturers doing this.
Utmost minimum is 50 micrometres, but with a high count of unrectifiable
rejects. I know one manufacturer.

200 micrometres with 0.4 mm bores is standard low cost. There is almost
no exemption.

Greetings
GerhartH
 
On 23 Feb 2007 01:33:59 -0800, "colin_toogood@yahoo.com"
<colin_toogood@yahoo.com> wrote:

What I am trying to understand is for a certain track and gap what via
size I should use. Presumably the two go hand in hand so that if a
design doesn't quite fit I would be able to reduce both for the same
incremental rise in costs but all I find is "ideally use this" and
"worst case we can cope with this" but the grey area between doesn't
get a mention.

Colin
Click to expand...
At some time in a previous century, the board shop charged extra
because I had specified 24 thou vias instead of my usual 25 - this
made me standardize on 25 thou. However, the board shops I use are
now willing to go down to 16 thou or less at no extra charge -
however, from habit, I still stick with 25 thou unless I really need
to conserve space.

--
Peter Bennett, VE7CEI
peterbb4 (at) interchange.ubc.ca
new newsgroup users info : http://vancouver-webpages.com/nnq
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top