Requesting help from EAGLE PCB users

[techie_alison]

Hello,

Please may I request help from an Eagle PCB designer users out there?
What's confusing me is if my design is suitable for submission to a PCB
manfacturer in Gerber format. I see alot of manufacturers quoting 2 layer
boards for 1 price, then 4 layer boards etc. etc. I'm guessing this refers
to multi layered boards with additional tracks sandwiched inside the board?
But using Eagle it also refers to layers such as top, bottom, pads, holes
etc. etc. These wouldn't each count in PCB terms would they?

Here is a .jpg of my design; http://www.retro.dial.pipex.com/pest/pest.jpg

It's very simple in that it has a single 18pin DIL on the topside, an SMD
smoothing capacitor on the underside. A 9pin D-type solders onto the side
of the board on the left. Signal wires from a cable go through the holes
directly next to the DIL on the right. The three large holes on the far
right take the main cable through the middle hole, with a cable tie nipping
the cable securely to the board. Space is absolutely critical given it's
obvious small size. I've copied this from the remaining boards I have here.

Here is the current .brd file if you would be willing to have a look;
http://www.retro.dial.pipex.com/pest/PeST.brd

I'd be extremely grateful for any assistance or pointers if I'm going wrong
as I've been dropped in the deep end since my working partner (who does the
electronics side) has started a regular paid job. And yes, I'm a girlie,
and no I'm not an electronics engineer, I'm an embedded software developer.
The prices we were used to paying were about £80 for 100 or so boards, and I
was quoted £700 odd pounds by a company today who want to do a complete
redesign when I already have a product. We used to regularly have prototype
runs from my partner's original company which has folded.

I have several other projects in the pipeline so it would be brilliant to
get these gerber files produced properly as soon as I can.

Thanks kindly,

Alison

 

[nappy]

Hello,

Please may I request help from an Eagle PCB designer users out there?
What's confusing me is if my design is suitable for submission to a PCB
manfacturer in Gerber format. I see alot of manufacturers quoting 2 layer
boards for 1 price, then 4 layer boards etc. etc. I'm guessing this
refers
to multi layered boards with additional tracks sandwiched inside the
board?
But using Eagle it also refers to layers such as top, bottom, pads, holes
etc. etc. These wouldn't each count in PCB terms would they?

Eagle has a good doc on multilayer boards in their help file I believe. .
Inner layers are usually Gnd & Power for a typical 4 layer board. If you
don't have those layers in your design you will have to add them. In my
designs they are layers 2 and 15.

 

[nappy]

ps.. also see the CAM OUT help files. There is a Gerber274x ( I think) job
file already setup . Use that as a starting point. In the CAM output dialog
you will be assigning your Eagle PCB layers to Gerber files. See how they
did it in the Gerber274x job ffile that came with Eagle.

 

[techie_alison]

Eagle has a good doc on multilayer boards in their help file I believe. .
Inner layers are usually Gnd & Power for a typical 4 layer board. If you
don't have those layers in your design you will have to add them. In my
designs they are layers 2 and 15.

Ok, ta

Am still tempted to go for a 2 layer board to keep the costs down, and that
there's almost nothing on the board so nothing complex. It does sound like
a good idea, quite impressed that it's now available to hobby prototypers.
What about VIAS? may I ask

But going to check out your other post about the help multilayer bit, on a
deadline here as been a bit stitched up. But will check out the help files
a bit more, just always been used to learning from others interactively.

 

[Tim Wescott]

Hello,

Please may I request help from an Eagle PCB designer users out there?
What's confusing me is if my design is suitable for submission to a PCB
manfacturer in Gerber format. I see alot of manufacturers quoting 2 layer
boards for 1 price, then 4 layer boards etc. etc. I'm guessing this refers
to multi layered boards with additional tracks sandwiched inside the board?
But using Eagle it also refers to layers such as top, bottom, pads, holes
etc. etc. These wouldn't each count in PCB terms would they?

Here is a .jpg of my design; http://www.retro.dial.pipex.com/pest/pest.jpg

It's very simple in that it has a single 18pin DIL on the topside, an SMD
smoothing capacitor on the underside. A 9pin D-type solders onto the side
of the board on the left. Signal wires from a cable go through the holes
directly next to the DIL on the right. The three large holes on the far
right take the main cable through the middle hole, with a cable tie nipping
the cable securely to the board. Space is absolutely critical given it's
obvious small size. I've copied this from the remaining boards I have here.

Here is the current .brd file if you would be willing to have a look;
http://www.retro.dial.pipex.com/pest/PeST.brd

I'd be extremely grateful for any assistance or pointers if I'm going wrong
as I've been dropped in the deep end since my working partner (who does the
electronics side) has started a regular paid job. And yes, I'm a girlie,
and no I'm not an electronics engineer, I'm an embedded software developer.
The prices we were used to paying were about £80 for 100 or so boards, and I
was quoted £700 odd pounds by a company today who want to do a complete
redesign when I already have a product. We used to regularly have prototype
runs from my partner's original company which has folded.

I have several other projects in the pipeline so it would be brilliant to
get these gerber files produced properly as soon as I can.

Thanks kindly,

Alison

When a board manufacturer talks about "layers" they mean the number of
layers of copper -- so a "2 layer" board is a single piece of insulator
with copper on top & bottom, where a 4-layer board has four layers of
copper, etc.

PC board software talks about silk, dimension, etc., layers. These
aren't 'real' layers in the sense of copper. The only ones that really
matter are the dimension layer, which the board house will want to use
for cutting out the board, plus the top & bottom solder mask and the top
& possibly bottom silkscreen for component legends. If you're doing a
quick-turn board you can often save money and time by leaving out the
silk and solder masks -- you get a board that's a bit harder to work
with, but much less expensive and with a shorter turn around.

Hopefully someone will direct you to a good company in the UK. Here in
the US I use PCB Express: http://www.pcbexpress.com/. While you don't
want to have stuff shipped from Oregon, their site may help you figure
out what questions to ask, and their guidelines are pretty good for just
about any board house. Somewhere on there they have a link to a free
Gerber viewer that you can use as a last minute check to make sure that
your output was sensible.

--

Tim Wescott
Wescott Design Services
http://www.wescottdesign.com

Posting from Google? See http://cfaj.freeshell.org/google/

 

[Tim Wescott]

Ok, ta

Am still tempted to go for a 2 layer board to keep the costs down, and that
there's almost nothing on the board so nothing complex. It does sound like
a good idea, quite impressed that it's now available to hobby prototypers.
What about VIAS? may I ask

But going to check out your other post about the help multilayer bit, on a
deadline here as been a bit stitched up. But will check out the help files
a bit more, just always been used to learning from others interactively.

You do _not_ need more than 2 layers! Most board houses do plated
through holes as a matter of course (do check, of course). As long as
the board house is plating through its holes and you are making your via
holes big enough for the board house they will work..

--

Tim Wescott
Wescott Design Services
http://www.wescottdesign.com

Posting from Google? See http://cfaj.freeshell.org/google/

 

[nappy]

also.. freedfm.com is very handy for checking boards before submitting
them.. to advanced circuits in Texas.

 

[larwe]

manfacturer in Gerber format. I see alot of manufacturers quoting 2 layer
boards for 1 price, then 4 layer boards etc. etc. I'm guessing this refers
to multi layered boards with additional tracks sandwiched inside the board?
But using Eagle it also refers to layers such as top, bottom, pads, holes
etc. etc. These wouldn't each count in PCB terms would they?

Look at the help for the CAM processor, it tells you what layers are
turned on for which output files.

For a 2-layer board, you will wind up with at least the following:

- drill CNC control file
- top copper
- bottom copper

If your design requires it, you might also have:

- top soldermask
- bottom soldermask

If your cosmetic sense demands it, you might also have:

- top silkscreen
- bottom silkscreen

If your design requires a SMD stencil, you might also wind up with

- top solder paste ("tCream and bCream")
- bottom solder paste

And so on. All those files are RS274-X Gerbers except for the CNC file,
which will usually be an Excellon file.

The "layers" in EAGLE are logical names referring to entities you might
want to turn off and on for visibility reasons; they have nothing
directly to do with the physical layers on the PCB.

I can send you a sample CAM job control file that outputs all the
correct files for a 2-layer PCB with silkscreen on one side and
soldermask on both sides, if you like. The procedure is then:

- RUN drillcfg.ulp to generate the drill list for your board. Save this
in a convenient directory
- Open CAM processor
- Load CAM job
- Edit paths for output files and make sure the drill page references
the drill list file you saved in the first step
- Click "Process Job"

 

[JeffM]

...help from an Eagle PCB designer users out there?

Alison (techie_alison)

I think you got most of your points covered, but the place
where you find the highest concentration oF EAGLE knowledge is:

Inside-the-loop Cadsoft guys (Employees)[1]

(Odd name--considering developments since Usenet started,
but I think you get the point)[2]

Since you're using something that kinda resembles a newsreader,
you should try to access them.
..
..
There is also a group here:
http://groups.yahoo.com/group/eaglecad/
..
..
[1] Others are free to recommend solutions as well.
[2] You get crossover from the factory guys here as well.

 

[Steve at fivetrees]

The prices we were used to paying were about £80 for 100 or so boards, and
I
was quoted £700 odd pounds by a company today who want to do a complete
redesign when I already have a product.

Your original prices sound about right for lowish volumes. Having taken a
look at your jpg, I can't see anything obvious that would require a
redesign.

I use a company near Bristol for PCB design and manufacture:
http://www.smbdesigns.co.uk/

Maybe they can help. They have a clue.

Steve
http://www.fivetrees.com

 

[techie_alison]

You do _not_ need more than 2 layers! Most board houses do plated
through holes as a matter of course (do check, of course). As long as
the board house is plating through its holes and you are making your via
holes big enough for the board house they will work..

--

Tim Wescott
Wescott Design Services
http://www.wescottdesign.com

Posting from Google? See http://cfaj.freeshell.org/google/

Okies, understood

 

[techie_alison]

When a board manufacturer talks about "layers" they mean the number of
layers of copper -- so a "2 layer" board is a single piece of insulator
with copper on top & bottom, where a 4-layer board has four layers of
copper, etc.

PC board software talks about silk, dimension, etc., layers. These
aren't 'real' layers in the sense of copper. The only ones that really
matter are the dimension layer, which the board house will want to use
for cutting out the board, plus the top & bottom solder mask and the top
& possibly bottom silkscreen for component legends. If you're doing a
quick-turn board you can often save money and time by leaving out the
silk and solder masks -- you get a board that's a bit harder to work
with, but much less expensive and with a shorter turn around.

Hopefully someone will direct you to a good company in the UK. Here in
the US I use PCB Express: http://www.pcbexpress.com/. While you don't
want to have stuff shipped from Oregon, their site may help you figure
out what questions to ask, and their guidelines are pretty good for just
about any board house. Somewhere on there they have a link to a free
Gerber viewer that you can use as a last minute check to make sure that
your output was sensible.

--

Tim Wescott
Wescott Design Services
http://www.wescottdesign.com

Posting from Google? See http://cfaj.freeshell.org/google/

Yep, am visualising it in terms of the early PC motherboards which were
originally 2 layer (original IBM PC 256K) and then went to 4 layer, and
wherever they are now (8, 16 layer). ie. when one looks at the side of the
board you can see the multiple sandwiches.

Would definitely go for a top and bottom silkscreen, not entirely clear on
the solder masks though.

Regarding companies who make up PCBs while looking on the Eagle site last
night found dozens (some in the UK) who prototype straight from the .brd
files produced by Eagle. Their prices are quite competitive with sample
quotes, ie. 2 160x100 PCBs = £50 with 10ish day turnaround.
http://www.cadsoftusa.com/Boardhouses/

The other thing that's crossed my mind is approaching a local educational
college, who often have the required equipment. I'll write over a letter to
see if they'd like to give some students the opportunity to make a few ££ as
well as the college.

 

[techie_alison]

Look at the help for the CAM processor, it tells you what layers are
turned on for which output files.

For a 2-layer board, you will wind up with at least the following:

- drill CNC control file
- top copper
- bottom copper

If your design requires it, you might also have:

- top soldermask
- bottom soldermask

If your cosmetic sense demands it, you might also have:

- top silkscreen
- bottom silkscreen

If your design requires a SMD stencil, you might also wind up with

- top solder paste ("tCream and bCream")
- bottom solder paste

And so on. All those files are RS274-X Gerbers except for the CNC file,
which will usually be an Excellon file.

The "layers" in EAGLE are logical names referring to entities you might
want to turn off and on for visibility reasons; they have nothing
directly to do with the physical layers on the PCB.

I can send you a sample CAM job control file that outputs all the
correct files for a 2-layer PCB with silkscreen on one side and
soldermask on both sides, if you like. The procedure is then:

- RUN drillcfg.ulp to generate the drill list for your board. Save this
in a convenient directory
- Open CAM processor
- Load CAM job
- Edit paths for output files and make sure the drill page references
the drill list file you saved in the first step
- Click "Process Job"

Brilliant info!! thank you If I can avoid Gerbers I may just go with
these boardhouses which can take straight .brd files. Thinking about your
offer of a sample CAM file, am going to see how I get on today with
approaching these .brd companies in the UK.

 

[techie_alison]

...help from an Eagle PCB designer users out there?
Alison (techie_alison)

I think you got most of your points covered, but the place
where you find the highest concentration oF EAGLE knowledge is:

Inside-the-loop Cadsoft guys (Employees)[1]

(Odd name--considering developments since Usenet started,
but I think you get the point)[2]

Since you're using something that kinda resembles a newsreader,
you should try to access them.
.
.
There is also a group here:
http://groups.yahoo.com/group/eaglecad/
.
.
[1] Others are free to recommend solutions as well.
[2] You get crossover from the factory guys here as well.

lol, 'something that kinda resembles a newsreader', yep, Outlook, ermmmmmmm.

Found the groups last night on cadsofts site;
http://www.cadsoftusa.com/forum.htm

 

[techie_alison]

Your original prices sound about right for lowish volumes. Having taken a
look at your jpg, I can't see anything obvious that would require a
redesign.

I use a company near Bristol for PCB design and manufacture:
http://www.smbdesigns.co.uk/

Maybe they can help. They have a clue.

Steve
http://www.fivetrees.com

thanks Steve

that £700 figure I think they thought I was some desperate dizzy dolly bird
without a clue (erm..).

going to get the .brd corrected today and send out for a few lowish quotes.

 

[Paul Carpenter]

On Tuesday, in article
<[email protected]>

....
....

Yep, am visualising it in terms of the early PC motherboards which were
originally 2 layer (original IBM PC 256K) and then went to 4 layer, and
wherever they are now (8, 16 layer). ie. when one looks at the side of the
board you can see the multiple sandwiches.

Would definitely go for a top and bottom silkscreen, not entirely clear on
the solder masks though.

Considering you have what looks like only 1 capacitor on the bottom of the
board I would only bother with doing a

2 sided PCB
both sides solder mask
(makes soldering the components easier)
top side silkscreen ident
(mainly so the chip can be orientated correctly)

This at places like pcb-pool <http://www.pcbpool.com/> is a fairly standard
and cheap variant and would be pretty good prices for your board size. Not
doing the solder masks on both sides does drop the cost further.

Regarding companies who make up PCBs while looking on the Eagle site last
night found dozens (some in the UK) who prototype straight from the .brd
files produced by Eagle. Their prices are quite competitive with sample
quotes, ie. 2 160x100 PCBs = ?50 with 10ish day turnaround.
http://www.cadsoftusa.com/Boardhouses/

Quite a few do a faster turnaround than that, however get quotes from
each of them (quite a few do it online) for the whole PCB supply including
tooling.

The other thing that's crossed my mind is approaching a local educational
college, who often have the required equipment. I'll write over a letter to
see if they'd like to give some students the opportunity to make a few ?? as
well as the college.

Depends on the college, and they don't work on the same type of deadlines
as you do, they are more likely to be interested if they can design the
circuit and/or layout as well. I would only approach them if the job was
not time critical in any way.

 

[techie_alison]

...
Considering you have what looks like only 1 capacitor on the bottom of the
board I would only bother with doing a

2 sided PCB
both sides solder mask
(makes soldering the components easier)
top side silkscreen ident
(mainly so the chip can be orientated correctly)

This at places like pcb-pool <http://www.pcbpool.com/> is a fairly standard
and cheap variant and would be pretty good prices for your board size. Not
doing the solder masks on both sides does drop the cost further.

Quite a few do a faster turnaround than that, however get quotes from
each of them (quite a few do it online) for the whole PCB supply including
tooling.


Depends on the college, and they don't work on the same type of deadlines
as you do, they are more likely to be interested if they can design the
circuit and/or layout as well. I would only approach them if the job was
not time critical in any way.

--
Paul Carpenter | [email protected]
<http://www.pcserviceselectronics.co.uk/> PC Services
<http://www.gnuh8.org.uk/> GNU H8 & mailing list info
<http://www.badweb.org.uk/> For those web sites you hate

Hi Paul,

Thanks for replying. I'm waiting to hear back from 4 companies at the
moment to see what they come up with. They have the .brd and the images
below.

To save further debate, here's my original PCBs;
http://www.retro.dial.pipex.com/pest/pest_top.jpg and
http://www.retro.dial.pipex.com/pest/pest_bot.jpg . The fresh .brd is now
here; http://www.retro.dial.pipex.com/pest/pest.brd

Truth is I haven't the faintest idea what the specs are for those boards in
PCB terms. They're about 25mm x 30mm, and I'm guessing with soldermask, and
top silkscreen.

What I'm really trying to do is to get as many for as little ££ as possible.
I guess the silkscreen (lettering) could go, not important. We were paying
about £80 for about 100 of those boards in 2 weeks or so. I've put this to
the 4 companies I've emailed.

It'd be great if anyone could tell me what the specs of these boards are.
Sorry to be a thick on this, this is a learning curve.

Thanks,

Aly

 

[techie_alison]

I've just been quoted £300 for 100 boards, what a bloody rip-off!! We were
paying £80 before.

 

[Steve at fivetrees]

I've just been quoted £300 for 100 boards, what a bloody rip-off!! We
were
paying £80 before.

That almost certainly includes non-recurring charges such as photoplots and
tooling. Maybe get a quote for repeat orders? That would give you a better
comparison.

Steve
http://www.fivetrees.com

 

[Spehro Pefhany]

I've just been quoted £300 for 100 boards, what a bloody rip-off!! We were
paying £80 before.

Your order would be considered down in the nuisance range by many
production board houses, so you just have to find one or two among the
thousands out there that want your kind of business. At this level,
the cost is really dominated by setup costs, not by board area. Some
suppliers are set up to do tiny prototype level orders, others want to
churn out more stuff. Your 100 boards will just about fit in a padded
envelope! No forklift required..

Specs for the board? You have to be a bit careful- if you underspecify
you may get bad results, if you overspecify the price may go up or you
may get no-bids or "go away" quotes. You'll get enough of those
anyway.

Try something like:

FR-4 material, double-sided with plated through holes
Board dimensions (INCLUDING THICKNESS**)
Solder mask both sides
Silk screen one side
<BOARD FINISH>*
NO testing required+

+I don't think it's worth it on such a simple board in such low
quantities... (but it looks like your assembled version almost has a
top-layer short between the microcontroller pin 13 pad and an adjacent
trace). When you get the boards, lay them out on a light table and
100% visually inspect each one before assembly. It will only take a
few minutes and you'll save much potential heartache.

* You might want to request quotes on what the board house suggests
for finish. There are trade-offs between cost, RoHS compliance,
solderability, bare board shelf-life and so on. If the supplier is
local, you can pick up the phone, or just ask for most economical or
something like that.

** Thickness is fairly important in your application as it has to fit
between the pins on the connector. Use digital calipers, or a
micrometer or something accurate like that.



Best regards,
Spehro Pefhany