1st Time PCB Design

There are a lot of suppliers around the $100 mark, depending on speed, how many you want, and shipping method/speed.

Single-sided means no vias and traces only on one side.

All holes (including those in footprints).

Do pay atention to the minimum trace size, minimum hole size (eg. for vias), and minimum annular ring..

Best regards, Spehro Pefhany

--
"it's the network..."                          "The Journey is the reward"
speff@interlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com

Hi,

Single side does indeed mean that all of the traces are on one side. Typically, jumpers are used in situations where things just won't work otherwise.

For an absolute beginner on a budget, one option is Their software seems to provide the necessary guidance for the beginner, and the ordering process is seamless. A typical beginner mistake is to send gerbers in the wrong format, resulting in a board that is 2.54 times too big.

Hope that helps, G.

Yes. Copper only on one side, no plated through holes.

Right.

It is.

It refers to and and all holes on the board.

One of the nice things about Olimex (for me and other Eagle users at least) is that they accept Eagle PCB project files directly, so there's no need to generate multiple Gerber files with different layers and drill tapes and whatnot. [Generating the proper Gerber files is probably the place where the most problems happen for beginners.]

Note that Olimex's minimum line width for the silkscreen layer is larger than the default line width in many layout packages (including Eagle). IIRC correctly, there was a macro package I downloaded from Cadsoft's site that you can use to fix up the silkscreen line widths before submitting the file to Olimex.

--
Grant Edwards                   grante             Yow! I'm also pre-POURED
                                  at               pre-MEDITATED and
                               visi.com            pre-RAPHAELITE!!

benn wrote in comp.arch.embedded:

If you can find a college/university/institute of technology near you, you could go in to one of the electronics technicians and ask could they send along one circuit board design with the rest of the students' project designs. Obviously they won't pay to get 50 thousand of them made for you but if you're only looking for one and if you explain to them that you're just doing it as a hobby then they'd more than likely help you out. My own college is great for things like that; we use the ".pcb" files that come out of Protel.

--
Tomás Ó hÉilidhe

Thanks.. yep I only need one, but Id like to go with a pay service just to get familiar with it in case I ever need to something like this again!

Im a software guy, but have access to Protel at work (actually we have a server license but I can connect to my work computer from home!). Anyways, I noticed Olimex and BatchPCB seem to prefer Eagle files, which I don't have. Are "Gerbers" a universal standard that most PCB places accept? Olimex only says it needs:

# Input file for TOP copper layer. # Input file for BOTTOM copper layer. # Input file for TOP solder mask layer. # Input file for BOTTOM solder mask layer. # Input file for component print layer. # NC drill file(s) for NC XY coordinates and Drill tools sizes. Note that the drill sizes should be the tool sizes used for drilling i.e. after plating your finished holes will be decreased with 0.1 mm

However, from the gerber output selection (

g ), it generated the following project output files: .rul, .rep, .gts, .gtp, .gto, .gtl, .gpt, .gpb, .gm1, .gg1, .gd1, .gb= s, .gbp, . gbo, .gbl, .extrep, .apr, .apr_lib which Im assuming are more gerber files than I need? Which options should I have checkmarked?

Thanks!

but not sure which of these files my 2 signal layer board shows these gerber output available:

go to

and download the free gerber viewer, which may give you a bit more confidence

martin

In case you want to give it a try, Eagle is free for hobby use (limited board size):

Yes.

Good question. The "Layer Names" arent using the standard terminology I'm familiar with. I'm guessing the "Top Layer" and "Bottom Layer" are the top/bottom copper layers. You'll have look at the protel docs to figure out what it uses for layer names for the solder-mask and for the silk-screen (print) layers. As somebody else suggested, you can use a gerber viewer to look at the files to see what they are.

It looks like you'll also need to generate drill files using the "Drill Drawing" tab.

There's all sorts of useful information on the Olimex web site (read the FAQ). There's a tutorial with step-by-step instructions on how to generate the proper files from Protel:

--
Grant Edwards                   grante             Yow!  I feel partially
                                  at               hydrogenated!
                               visi.com

Yup. BatchPCB has a pretty good FAQ:

*+Excellon-*-*-*+requests+proprietary+Gerber+Drill.file+Gerbers&strip=1 You will need Gerber and Excellon (drill) files for most fab houses.

These guys do plated-through (2 sided) boards at reasonable prices. Quality is excellent.

John

Thanks, I'll definitely look into it. Im not set on Olimex, I just thought they were reasonably priced. The others I had looked at were:

Im sure they're all pretty much the same, but would like to go with one thats a bit more tolerant on a newbie and maybe even check my design to make sure I didnt do something dumb :)

I like

For single boards they're a bit more expensive than olimex, but the prices drop quickly for moderate quantities, which is nice if the board works and you want to make a batch of them without changing suppliers.

I also like their 6 mil traces/clearance, as well as their 0.25 mm holes.

Another endorsement for Alberta. The "how to submit your order" walk-through and clear layout requirements worked well; good boards on the first try.

If you don't need the boards *quite* as fast, another place to look is the batch option from the Sparkfun guys at

The tutorials at

may also be of interest.

If you go the Gerber route (nice, in that it means vendor independence) you'll want/need a viewer. Among the free ones out there you might want to give

a try.

--
Rich Webb     Norfolk, VA

Don't forget that Olimex hole sizes are non-plated. If you have a PTH double-sided board you need to allow for this, otherwise your holes will be too small.

Leon

Thanks! I missed that little detail on their site!

The Gerber export tutorial shows how to set the drill options, but I think this only sets how the drill information / gerbers are rendered, but doesnt actually set any design changes. Is this right, does the PTH / NPTH drill information need to be explicitly defined elsewhere (not just in the gerber output settings) prior to routing?

Also, if they dont plate the holes wouldnt it just make the hole a bit roomier than if were plated? Since the footprint calls out for a particular thru-hole ic, even if theres wiggle room, as long as I solder on both sides of the board, it should be ok, no? I guess Im not sure whats the idea behind plated thru holes?

I don't know about your cad program, but in general you tell the cad program that each hole is plated or non-plated, and it eventually spits out two drill files - one for all plated holes, one for all non-plated holes.

I usually make my holes 5+ thou over the physical size, so the 1-2 thou that plating adds isn't a problem.

Two reasons: 1. the size is more precise, and 2. you don't need a copper annulus around it, so the thickness and flatness of the PCB at that point is more predictable.

Use plated holes when you're electrically connecting something. Use non-plated holes when needed for mounting and mechanical holes.

If you can get away with only plated holes, it may be cheaper. Non-plated holes means an extra manufacturing step, plated holes are "standard".

As for why they're needed - you can't always get to both sides. Think of a radial lead 1000uF capacitor - the cap covers the copper when plugged all the way into the board, there's no way to get in there with a soldering iron.

But you can get away without plating, such as when home-brewing boards, if you carefully plan all your traces so they're always in a solderable location.

Hole sizes are output in the Excellon drill file, which is similar to other CNC machine control file. It is an ASCII file that looks something like this:

(I've replaced a bunch of similar lines with ... below).

% T1C0.020F200S100 X001750Y008600 .. X023500Y019000 X028250Y008750 T3C0.035F200S100 X012000Y017500 .. X027000Y006750 T2C0.034F200S100 X012000Y023500 .. X023550Y007750 T5C0.054F200S100 X025000Y009250 X026000Y008250 X027000Y009250 T9C0.143F200S100 X002000Y002500 X002000Y022500 X026000Y015200 X027000Y002500 X027000Y022500 T8C0.128F200S100 X016250Y005390 T7C0.108F200S100 X014480Y004210 X016250Y003030 X018020Y004210 T4C0.040F200S100 X001250Y011000 ... X001250Y018000 T6C0.057F200S100 X006500Y002000 X008500Y002000 X010500Y002000 X012500Y002000 M30

This one is in inches. The lines beginnning with "T" are tool definitions (I think the associated feed rates and spindle RPM definitions are usually ignored or replaced). The first one (T1) is a

20 thou via drill. Each line beginning with X is a hole location (X, Y in inches with 0.0001" resolution).

You can manually edit this kind of file to alter the drill sizes a bit, but it's best done very carefully, if at all, and checked with a viewer later to make sure that you've not introduced design rule violations such as drilling away too much of the pads.

Typically the hole sizes are *defined* in the footprints.

On prototype PCBs often all the holes are plated through. To make some holes unplated costs more because it's a separate operation- and typically a separate drill file is generated, either automatically or by the vendor. It's not uncommon on production boards to specify some holes as unplated (eg. mounting holes or snap-in holes for connectors).

Best regards, Spehro Pefhany

--
"it's the network..."                          "The Journey is the reward"
speff@interlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com

Yup. That's why the call them "drill sizes" not "finished plated hole sizes".

They connect traces on opposite sides of the board to be connected. Traditionally, one only solders one side of the board.

I don't think most vendors have an options for non-plated holes on double-sided boards.

--
Grant

d l e

They do plate the holes, of course. You have to allow for the plating thickness.

Leon