Instructables

Professional PCBs almost cheaper than making them at home

Picture of Professional PCBs almost cheaper than making them at home
While there is great satisfaction in home building PCBs, adding up the cost of the blank PCB, etchant and the drill bits comes to over $4 per board. But for $6.25 a board the whole thing can be made professionally. This Instructable takes you through the steps to create the Gerber files that the PCB manufacturers need. The total cost was $75US including shipping for 12 boards. 3 boards would be about US$62.

This Instructable builds on some great work at http://www.instructables.com/id/EXU9BO166NEQHO8XFU (Draw Electronic Schematics with CadSoft EAGLE) and http://www.instructables.com/id/EZ3WN1QUKYES9J5X48 (Turn your Eagle schematic into a PCB). Eagle is free.
 
Remove these adsRemove these ads by Signing Up

Step 1: Designing the schematic

Picture of Designing the schematic
The full schematic is at http://drvernacula.topcities.com/315_mhz_solar_powered_radio_rptr.htm and is the schematic for a solar powered radio repeater module.

Step 2: Place all the components

Picture of Place all the components
The instructable links on the intro page show how to create a pcb from a schematic using EaglePCB. One main difference is that none of the design rules about track widths need to be changed at all (the drc design rule check). The defaults are all fine and while the tracks look really thin and close to pads it doesn't matter as the green solder mask makes it very easy to solder. In fact, these sorts of boards are much easier than soldering up prototypes. Some big pads were used for connecting external wires and there were a few extra comments added for the white component overlay layer.

The wonderful thing about having boards like this made compared with building homemade boards is you don't have to worry about trying to optimise the autorouter for a single layer. Just run the autorouter once and it defaults to double layer mode and it always produces a 100% design automatically within a few seconds. Even with components a lot denser than this board Eagle always autoroutes the whole board.

Step 3: Fix any errors

Picture of Fix any errors
Sometimes one finds a better component in the library or changes a component. To rip up and replace the tracks click on the ripup symbol (green circle), click on the traffic light (red circle) and then reroute (yellow circle).

Over the last few years I've found a few tips and tricks to making better boards:
1) To get tracks closer - Tools/Auto/General and set the grid to something like 10mil
2) To make data tracks thin but power tracks fatter, Edit/Net (at the bottom) and start typing in a text box to name the class. I use three classes; Gnd, Power and one for all the rest.
3) In DRC, distance/copper dimension change from 40 to 20 - this allows two tracks to fit between IC pads, which can greatly increase board density.
4) In DRC - clearance/pad to via increase from 8 to 40. (leave all the rest at 8mil). This increases the distance between vias and pads so less chance of bridges when soldering. Surprisingly, this also sped up the autorouter too.

Step 4: Create a drill file

Picture of Create a drill file
The manufacturer needs to know what drills to use. Eagle has automatically used whatever drill fits the components that have been chosen. Go to File/Run and select the file "drillcfg.ulp". I selected inches rather than mm and that seemed fine with the manufacturer. Click ok then ok again. It will save a file with a .drl extension.

Step 5: Create an Excellon drill data file

Picture of Create an Excellon drill data file
Click File/Cam Processor

Step 6: Open the Cam Processor

Picture of Open the Cam Processor
In the Cam Processor click File/Open/Job

Step 7: Select the Excellon File

Picture of Select the Excellon File
Select Excellon

Step 8: Click on Process Job

Picture of Click on Process Job
Click on Process Job. This will create some files. Close down this menu with the x at the top right.

Step 9: Create the Gerber files

Picture of Create the Gerber files
Repeat steps 5) and 6) to reopen the CAM processor and this time open the file gerb274x

Step 10: Create the Gerber files

Picture of Create the Gerber files
This is the important bit. You need to click on each one of the tabs circled in green and ensure that Mirror (circled in yellow) is off. As you click through the tabs you will notice the Nr and Layer lines highlighted on the right will change. One default you might want to change is component values - in my copy this was deselected and the silk screen ended up with U20 but not the actual chip - eg an IC might be 74HC04. Click along the tabs to Silk Screen Cmp, and click on 27 tvalues. Once all the mirror boxes are definitely unchecked, click on Process Job (red circle).

Step 11: Collect all the files and Zip them up

Picture of Collect all the files and Zip them up
I collected 10 files, put them in a temp directory and used winzip to create a single zip file. I have a feeling that one or two of these are not actually needed by the manufacturer but I sent them anyway. The file the manufacturer definitely does not need is the .sch schematic file.

Steps 4-11 are summarised in text format at http://drvernacula.topcities.com/creating_gerber_files_from_eagle.htm

Step 12: View some of the files just to make sure

Picture of View some of the files  just to make sure
Download a free Gerber file viewer

Step 13: View a Gerber file

Picture of View a Gerber file
The drill files can be viewed with a text editor.

The Gerber files can be viewed with a free Gerber file viewer. I went to the website above and installed Viewmate. It appears in the Start menu of windows as Start/Programs/Pentalogic. In Viewmate I clicked on File\Open and browsed to C:\Program Files\EAGLE-4.16r2\projects\RadioRepeater and at the bottom of the windows changed Files of Type to *.*. As an example this is the .sol solder side file

Step 14: Find a PCB manufacturer

Picture of Find a PCB manufacturer
This company OurPCB is in China and stood out from some of the others in that they freely advertised their price for small quantities. Shipping is FedEx and to the US they quote $22. The $40 above for a 10 sq inch board is for all the 3 boards, not per individual board. At a quantity of 100 the price per board is $1.80 each. They can give a firm quote once they get the zipped files.

These boards arrived in 9 working days. There were a few problems initially with me sending the wrong files (which is mainly why I wrote this Instructable!) and they were very patient and polite from their end. There were also some email problems in that emails coming back were totally blank. I was able to read the source text and at least work out who they were from but I nearly did delete the mail as junk mail. Finally I ended up communicating by Skype text. They all write very good English which is a bit embarrassing as my Mandarin is non existent. My kids are learning Mandarin at school though.

Payment was via Paypal which remains safer than using a credit card (for both parties) and far cheaper than an interbank transfer.

I hope this Instructable is useful. I have built many hundreds of prototype boards over the last twenty years but I think from now on I will be getting boards made professionally.
echoalex9 months ago
Hey, this is one instructable that I have been using as a reference material for the last 3 year, when ever I want to make a gerber file. I keep forgetting what to do while making a gerber file. I think its about time that I thank you. Thanks a bunch for this amazing instructable.
dosadi4 years ago
I'm surprised no one has mentioned SparkFun's batchpcb.com prototype service. They take small orders and combine them into panel orders that are processed by Gold Phoenix. 2 layer boards cost $2.50 per square inch with a $10 setup fee. They're slow, though. Expect to take at least 3 weeks while they gather together a batch order and transit from China, etc. Since they use Golden Phoenix to produce the boards, you already know GP will accept your files when you're ready for a larger batch.
The Portland Dorkbot group has been doing batch PCB orders every month for over 8 months, and recently opened it up to anyone. Basically, the cost is $5 a square inch and you get three copies of your board. 6mil traces and spaces, double sided, with solder mask and silk screen. I submit a board or two almost every month. This is perfect for Eagle CAD sized boards. Check it out at http://dorkbotpdx.org/wiki/pcb_order
And this guy accepts straight eagle files, so you don't even have to deal with gerbers at all. I had one run to get eighteen total boards that cost under $50. Granted twelve of those boards were really tiny (.7" diameter). I highly recommend this.
abraxas24 years ago
Thanks for taking me a leap forward. When I process this board into files via the CAM, I notice the check box "Fill Pads" is checked and I can't uncheck it because it's grayed out. Sure enough the artwork in the files generated has all of the pads filled in. I'm doing home brew boards so I need these holes as a guide for my drill. Your help in unfilling these holes is appreciated.
siddhc abraxas22 years ago
Hi,

I also have the same problem .. "Fill pads" is checked and I cannot un-check it.

Please help if you figured out the solution.

Thank you very much,
DaleS442 years ago
My misteak! Roller microchips should read roller micro switches! The kind that are actuated by a cam. Is shaping the pc board and cutting slots for some of the components done by another device like a router (not trace router) that requires a separate instruction set?
DaleS442 years ago
I recently needed to build a simple PC board so I downloaded Eagle PCB. With the help of a couple of tutorials and your instructibles I was able to complete the project to the finished, and previewable, gerber files. Your step by step instructions made the process very seamless.
I have one question though. My PC board must have a u shaped cutout in the top of an otherwise rectangular board. I also need to mount some roller microchips on this side where there is an angle and very specific measurements between holes.
Is there a feature in Eagle PCB that allows more specific adjustments to the size of the board beyond pulling in on the side frames and is there a way to locate non-pad holes for mounting the micro switches so that they are in a very precise location and can be drilled when the boards are being manufactured? I do have the entire project in AutoCAD and I have a drill layout and shape as one of the layers. I am just unable to figure out how to export this layer in a format that can be combined with the output files from Eagle PCB.
Thank you for your help and for taking time to respond.
Dale
Dr_Acula (author)  DaleS442 years ago
Thankyou for the kind words.

I am not sure about changing the board shape but I think there are other instructables that might show how to do this. Search for Eagle? Also you would probably need to ok this with a PCB fab house. Maybe start with the PCB manufacturer first.

Re non pad holes, I have found it easiest to design a new part. There are instructables on how to do this. One of the things you can add to a new part is a hole (of various sizes). It helps to have the exact part dimensions.

Sorry I can't help further but there are other instructables written by authors who know a lot more about Eagle than me!

Cheers, James Moxham
This comment may be late in the game:

"always autoroutes the whole board"
Not true.
I have been creating Arduino-size PCBs (80x100mm, 60x80mm) with 3-4 extra SMD ICs, and Eagle has hard time completing it. One needs to take care with component placement or you find yourself having to clean up a lot.
Oddly, even with 2 ground planes, the place where I have been left hanging is ground connections! I've been having luck with that by moving signals around manually to let the lower & upper ground areas overlap and then adding a via to connect them.
I'm using the free eagle software, and have the 1-sheet schematic pretty full up, not a lot of interconnections shown to free up space, bunch of parts with just signal names hanging off.
hamraddude5 years ago
OurPCB sucks thundershit. I asked them for a quote on a 2.5 in x 4 in double sided PCB, and the price came up to 6.30 USD + 30 USD (!) shipping and 100 USD "tooling charge". Yep, 136.30 USD for a 2.5 in x 4 in double sided PCB. No thanks, I'll keep making my own.
For smaller scale you need a different PCB company. Different companies specialize in different things:
http://www.seeedstudio.com/depot/fusion-pcb-2-layer-10cm10cm-max-10pcs-p-396.html?cPath=64_12
http://iteadstudio.com/store/index.php?main_page=index&cPath=19_20

A quick price checker for these and the rest:
http://www.ladyada.net/library/pcb/costcalc.html

This one has a really good student offer, $33 for 3 boards with all bells and whistles I think
http://www.4pcb.com/

And of course they already mentioned sparkfun and some other sites that do single boards at a higher price.
Dr_Acula (author)  hamraddude5 years ago
Just double check that $100 - they tried to charge me that last month but it was because it was the Chinese New Year and I think they wanted a holiday. $50 is the usual charge. I think if you want just one board do it with a prototype. If you want 3, there may well be other manufacturers where the price is cheaper because you can piggyback on other people's orders. But if you want 10 boards or more, it ends up very good value IMHO. Tonight I'm sending off an order for 10 sprinkler controller boards and it works out good value, especially if I cost in my hourly rate building 10 prototypes with point to point wiring vs 1.5 hours designing a PCB. Maybe try searching for some of those other manufacturers that piggyback single orders.
guyfrom7up6 years ago
I beg to differ, 4 bucks a board? Maybe if you buy everything from radioshack. For me it costs about a dollar a board to make a t home.
Dr_Acula (author)  guyfrom7up6 years ago
It depends if you add in the setup fee and the shipping fee, which are fairly fixed regardless of how many boards. I just ordered another batch of 20 and the actual board cost was 23c each.
I found a seller on eBay who sells 360sq. inches of single or double sided, any thickness, any size blank copper clad board for $10 + $10 shipping. I got 60 boards, for $20, that's about $0.33 per board.

http://www.minute-man.com/acatalog/ sold me enough ferric chloride to last a lifetime for $20

My laser printer was $10 on Craig's List

I built a heated, agitated etching tank for $25.

So for $75 I can make 60 boards, that's a little over $1 per board, plus I only have to reorder the copper.

As far as ordering online, though, this is a pretty cheap site for small quantities, thanks. Great instructions on making the Gerbers, too!
how did you make the heated, agitated etching tank
Instead of that, you can also use pigmented ink, yellow is best (I guess it needs more pigment than other inks to look right), to act as a resist. You do need to watch etching times though.
http://www.inksupply.com/product-details.cfm?pn=MISPRO-4-Y
Hello,

I read the comments but confused about the low pcb costs.
For example, I am using ExpressPCB tools.
Cost of making 4 boards size of 4 * 5.5 inches is $ 269, professional services including solder mask and silk screen.
The standard service is $ 124 without solder mask and silk screen.
PCB manufactures say need gerber files, can't do it without.
The cost of gerber file order is $ 60.

Andrew
Dr_Acula (author)  amp07094 years ago
It certainly is worth shopping around for prices! On the last page is a link to OurPCB and they are a lot cheaper. I got 12 boards 11x16cm made recently for $110. And due to the fixed setup/shipping but very cheap actual board cost, I also recently got 30 boards 5x5cm for $89. That includes mask, screen etc. Yes they need gerber files, but this instructable shows how to make them (that doesn't cost anything and takes about 30 seconds once you know the shortcuts). I'm using Eagle and the free version can only make beer-coaster sized boards. But if you pay $125 once-off you can go up to a reasonable size. That pays for itself over only a couple of runs. I hope this helps :)
Does not cost only a dollar if you don't have all the stuff to do it. I can say for sure getting boards made is a lot cheaper than making them at home. I worked at a couple PCB fab places & got a ton of tooling & FR404 1/2 1/2. I have a mill & cut my own, but with time, forget it, just get 'em made. Right now Gold Phoenix is $99 for 155 sq in.
abraxas23 years ago
Again, a million thanks for your generousity in producing this fine tutorial. It's been a lifesaver !! One problem I am having at this point using both your tutorials, is that I am getting a solder image without pad holes for my components. They would be nice to guide my drill as I am making my own boards. THANK YOU !!!
Dr_Acula (author)  abraxas23 years ago
Great to hear it is helping someone! Can you provide some more information about the solder image? There is the .sol file but there are lots of other files produced. Are you making your own boards or sending them off?
I'm making my own. I followed the instructions to a Tee. I did all the steps but when I view the resultant .sol file, all the pads are filled in. when I print that sol file, likewise, no holes.
Dr_Acula (author)  abraxas23 years ago
The gerber files are for the fab house and splits up the board into lots of layers including the solder layer, top side, bottom side, text, and masks. So just bundle them up and send them to the fab house.

If you are making your own boards, then I think you need to print out the layers as a file/print rather than create gerber files.
smartroad4 years ago
Hi,

Having problems with the drill file, all I get as an output is:

T01 0.032in
T02 0.040in
T03 0.079in
T04 0.126in

and nothing else, so when it uploads to a PCB Fab they say the drill file doesn't exist. What am I doing wrong?
aimee473024 years ago
Thanks! I followed your tutorial to create my first gerber a couple of weeks ago! If you are looking for a good place for PCB manufacturer my Professor recommended PCB International (http://www.pcbinternational.com). We fit in 4 different parts and the total charge was only $94. We just recieved them a few days ago and they look great! 
TopJimmy4 years ago
I also like reading articles on homebrewing boards. A good source for PC boards and supplies is www.j-tron.com. Nice article. www.meltedsolder.com
This instructable is right on! It enabled me to create my files and the board came out perfectly. Thanks so much! Ali
ledsales5 years ago
I get all my boards done through Futurlec (www.futurlec.com) as they do a good job and only need the original PCB file, not all the separate files like gerber etc (this is the 21st century, about time PCB makers realised that getting boards made should be simple - it's not rocket science after all). They will email you a pdf of the various layers and masks etc before manufacture (make sure you ask for this) and if you become a regular like me, they may even do all your prototypes gratis, they do mine... The only thing to watch out for is that on multilayer boards, their drill sizes are the size of the hole they drill before they sleeve it, the finished board will end up with holes about 4 mil smaller than your drill sizes specified. Also, being based in Thailand, there can be a few language issues - just make sure you ask for that PDF proof!
Dr_Acula (author)  ledsales5 years ago
Good find! And a slightly weird experience as I was in the Futurlec site buying some leds when this message came through. (I just noticed your username - this is getting even weirder?!) They have an automatic quote system and for a 80x160mm double sided board, $74 for 1 board, $99 for 3 and $190 for 10. Plus $14 shipping. I like Futurlec - $4 shipping for small orders worldwide (vs $30 for digikey). Plus I emailed them once about adding a part to their stock and they added it a week later. Free protoboards? Nice. How does that drill size thing work? Does it mean that standard library files from, say, Eagle, end up not quite fitting standard components or is 4mil too small to notice, or do you just push the components in?
The Futurlec online quote system is pretty inaccurate, it always quotes higher than what they really charge you in my experience, so always email them (sales@futurlec.com or sales@futurlec.com.au for anyone in Oz) to get a quote...
ocayaro5 years ago
guyfrom7up try making a six layer board at home then
As a new Eagle user and being retired 12 years from design, this Instructable was a HUGE help. thanks so much for taking the time to put it together. mark
Of course the unseen costs need to be considered. Wiring an extremely complex board may take a long time and be fraught with errors. If the wiring takes you 2 extra hours per board and your salary is $20 an hour then you've saved $40 by avoiding hand wiring.
rpwilsonjr6 years ago
Thanks for the very useful Instructable. I followed it, submitted the CAM files to the OurPCB, and 10 days later I had PCBs in hand. I assembled two of the boards right away, and they worked.
UltraMagnus6 years ago
Eagle is not free at all, only a neutered beer free version is. GNU EDA is far better and entirely free
Dr_Acula (author)  UltraMagnus6 years ago
It is free for boards up to a little bigger than the one above. For big boards, yes it costs but many projects can be fitted on a board of this size.
as i said, only a neutered, or crippled version is "free"
Pro

Get More Out of Instructables

Already have an Account?

close

PDF Downloads
As a Pro member, you will gain access to download any Instructable in the PDF format. You also have the ability to customize your PDF download.

Upgrade to Pro today!