How to prepare your PCB files for order?
Please do always RUN DRC check before sending boards for production and do
not send boards for production which have errors. We can't manufacture boards
which fail DRC check and sending boards with errors for manufacturing just increase
your order delay and your price.
What you should make sure is:
- your board no overlaping drill holes;
- no copper tracks/pads spaced at less 8 mils (0.2 mm);
- not using drill holes under 0.6 mm and over 5.0 mm;
- your pads/vias are 0.4 mm bigger than your drill holes so there is 0.2 mm
copper ring around your drill holes;
Your soldermask openings are not above 20% of total panel area, our finish
is GOLD if there is no soldermask, or there are big soldermask openings we have
to charge you additionally, so to produce board without soldermask by our process
is more expensive than to produce board with soldermask, do not forget
to send your soldermask files;
- Make sure your panelization is possible i.e sending two boards with 100x80
mm and asking them both on 160x100 mm panel is not possible. Please read our
FAQ on panelization.
Note that if we receive PCB files with errors we will just waste time to process
and check them, then we will point you your errors, but we also will have to
charge you re-processing fee for your new PCB submission, to save our time and
your money please do DRC check before sending your boards for production!
Also we strongly encourage you to generate your Gerbers yourself and to check
them with gerberviewer, sometimes it's hard to notice some silly errors in your
CAD like printing component names or values over your SMT pads, note that we
do DRC check only on the copper layers, from PCB manufacturing point of view
it's not error if you cover your pads with soldermask or if you print over your
SMT pads, your boards will be produced exactly as you have designed them, but
you will have hard time later to solder them, so the best professional approach
is to generate your gerbers and check them before sending boards for production.
Good convention for file names are MYPCB-REV-XXX-DATE.zip as if you send us
several files with name PCB.zip or ORDER.zip and later you want to reffer one
of them we would not know which exactly PCB.zip out of the ten files with name
PCB.zip you sent us you do reffer to.
All PCB files should be accompanies with README.TXT as per our README.TXT
template, files which have no README.TXT will not be processed.
Note that all remarks and notes regarding your PCB manufacturing should be in
this README.TXT all other info or requirements outside this README.TXT aka sent
in your e-mail body or Gerbers or elsewhere is IGNORED.
We need the Eagle BRD file and README.TXT
as per our template. Please use the 8mils DRU to
DRC check your boards before sending for production.
Please do not send us Eagle BRD files made with cracked/illegal licensees
we can't open such boards so we can't manufacture PCBs made with such licensees.
Boards made with Eagle FREEWARE licensee are OK for manufacturing.
Note that when you send Eagle BRD file we use ONLY Eagle DEFAULT layers to process
your gerbers, these layers are: TOP: Layers 1, 17, 18; BOTTOM: Layers 16, 17,
18; SILK: Layers 20, 21, 25; TOPMASK: Layer 29; BOTTOM MASK: Layer 30. If you
put information on other layers please post-process the BRD file by yourself
and switch ON the layers you are using, then send us the Gerbers and NC drills
If you want to generate your Eagle PCB manufacturing files by yoursefl follow
this Eagle tutorial
***NEW*** Customer of ours wrote GREAT
Tutorial how to PANELIZE your Eagle boards together in panel and the
Target 3001 users
We need the T3001 BRD file and README.TXT
as per our template.
Please note that when you send T3001 BRD file we use ONLY DEFAULT layers to
process your gerbers, these layers are: TOP: Layers 16; BOTTOM: Layers 2; SILK:
Layers 21, 23; TOPMASK: Layer 18, 23; BOTTOM MASK: Layer 4, 23; If you put information
on other layers please post-process the BRD file by yourself and switch ON the
layers you are using.
If you want to generate your Target3001 PCB manufacturing files by yoursefl
follow this T3001 tutorial.
We need the BRD file and README.TXT as
per our template.
If you want to generate your KiCAD PCB manufacturing files by yoursefl follow
this KiCAD tutorial.
Other CAD users
We need Gerbers in RS274X format with embedded apretures any aperture sizes
above 8 mils is acceptable, precision should be 2.4 or 3.4. Please add border
outline to your Gerbers.
NC drill file in Excellon format with precision 2.4 or 3.4 with embedded drill
tool info and README.TXT as per our template.
Separate GERBERS should be generated for the TOP/BOTTOM Copper, TOP/BOT Soldermask
and TOP/BOT Component print layers.
Please have a look at the Protel
Tutorial which one of our customers wrote, or check our Eagle,
Target3001 and kiCAD
tutorials, generally the same rules apply for the other CAD products too.
- Our minimum track width/space is 0.2 mm (8 mils).
- The (pad/via - drill hole) clearence must be minimum 0.4 mm (16 mils) i.e.
the resulting annual copper ring around the drilled hole to be 0.2 mm (8 mils),
example: if 0.9 mm drill hole size is used it MUST have pad/via diameter =
min. 1.3 mm
- Our minimum drill size is 0.6 mm (24 mils). we can't manufacture boards
with smaller drill hole size.
- Our maximum drill size is 5.0 mm (197 mils) we can't drill large than 5.0
mm drill hole on your board, if your board have > 5.0 mm drill it will
be replaced with 5.0 mm drill
- Our standard drill tool rack is: 0.7 mm (0.028"), 0.9 mm (0.035"), 1.0 mm
(0.039"), 1.1 mm (0.043"), 1.3 mm (0.051"), 1.5 mm (0.059"), 2.1 mm (0.083"),
3.3 mm (0.13").
If you are using non-standard drill sizes you will be charged additionally
see our PRICE web page.
- We are using METRIC drill sizes with step of 0.1 mm and all drill sizes
are to be rounded to the nearest metric drill size. For instance if you are
using 27 mils, 28 mils and 29 mils drill sizes they all will be rounded to
0.7 mm. To convert from IMPERIAL to METRIC you should divide your IMPERIAL
drill size to 39.37 i.e. 130 mils / 39.37 = 3.3 mm and vice versa 1.0 mm =
39.37 mils after rounding = 39 mils. If this rounding is not taken into
consideration you can easily make DRC violations - for instance
you can use 34 mils drill with 50 mils pad/via which should pass the annular
ring copper check as the pad-drill is 16 mils, but 34 mils drill = 0.86 mm
will be rounded to 0.9 mm and the 1.27 mm pad/via will fail on the DRC check.
- Our drill hole limit is 500 holes for SSS,DSS and 2000 holes for SSQ,DSQ
panels. If you exceed the maximum hole limit you will be charged additionally
see our PRICE web page.
- Each layer MUST have text inside or outside PCB area to prevent board production
with mirrored layers. i.e. the text on bottom should be mirrored if you look
on the board from top.
- Lines under 0,1 mm (5 mils) on component print layer may not be visible.
MATERIALS WE USE FOR PCB PRODUCTION:
- Manufacturer: CKC TAIWAN
- ANSI grade FR-4
- Laminate thickness 0.5 mm, 0.8 mm, 1.0 mm, 1.5 mm
- copper 18 um (1/2 oz) or 35 um (1 oz)
- operating temperature Tg > 130 C
- soldering 260C/500F - 40 sec., 290C/554F - 20 sec.
- Dielectric cinstant 1Mhz: 4.0 - 4.5, guaranteed < 5.0
- Dissipation factor 1MHz: 0.02-0.03, guaranteed < 0.03
- Volume resistivity: Ohm.cm > 5*10^14
- UL 94V-0, UL746 CTI 100
Solder mask: SD2467DG
- LAMINAR 5000, manufacturer: Morton Electronic Materials Inc.
- Riston 200, manufacturer: Dupont Electronic Materials Inc.
- manufacturer: Lackwerke Peters GmbH
- UL 94 V-0, UL file: E80315