Category:PCB PCB Layout

Group Administrators: 1 | Group Member: 83 | Group Threads: 106

The connections on a PCB should be identical to its corresponding circuit diagram, but while the circuit diagram is arranged to be readable, the PCB layout is arranged to be functional, so there is rarely any visible correlation.

Thread Reply
Must-knows in Your Custom PCB Fabrication Drawing Reply 2017-02-18 09:11:45
1K+ views
1 comments
285 likes

linhpost

Leave A Message

Follow

Dealing with PCBs day in and day out gives us a lot of exposure to good and bad engineering drawings. It is rare that we come across engineering drawings that are complete enough to create a comprehensive quote. More often than not, a drawing is missing a key component that we must go back to a buyer and ask, “There were no specifications in your drawing for…..what do you want for this specification?”
If design engineers and layout engineers would simply create a bullet proof fabrication drawing, a significant amount of time and effort would be saved in the quoting, CAM and production process of creating a printed circuit board.
Below is a wish list of critical PCB specifications you should include to help your PCB Manufacturers get it right:
  1. Layer Count – this data can also be found in the Gerber files, however, a quality stack up on the fabrication drawing and even creating a note on the drawing always helps a CAM engineer confirm material types for both copper laminate and prepreg. It will also help the quoting person quickly compare FAB specs to the Gerber for quicker and more precise quoting.
  2. Material Type- the material call-out can be one of the largest variance specifications. It is one that should be called out correctly and some specific notes will help with an accurate quote. Most all materials these days default to FR4 mostly because of its UL Certification on flame ratings. Currently, it is by far the most popular material. There are times when companies want to shave off some price and go for the lowest price and they will call out FR-1, CEM-1, etc. However, there are few suppliers or manufactures stocking these lower flame rated materials. They have become almost non-existent except in extremely high volume production / fabrication. Back to FR-4 – An FR-4 material should have a call out for its TG rating or temperature rating. Bob explained briefly the how to decided on TG / TD ratings in a prior blog post. What is important from a quoting / engineering perspective is that the drawings and Gerber note “FR4 Tg135” material being called out. In today’s RoHS world, many RoHS assemblers want a higher Tg rated material and that should be noted as: “FR-4 Tg170” or “greater material required.” The key is to note it specifically so there is no guess work on what the PCB should be fabricated with. One might add “Material Flammability Class shall be approved to a minimum of 94V-0.” This is really generally accepted these days but we do see it on very detailed drawings.
  3. Beginning Copper Weight- options for starting copper weight can be .5oz, 1oz, 1.5oz et cetera. Sometimes this matters to the engineer and helps the PCB manufacturer understand what base material the customer wants.
  4. Finished Copper Weight- This is more critical than the beginning copper weight because it lets the fabricator know specifically what the finished copper thickness needs to be – just stating the obvious here. It should also be noted that each layer needs to be designated if they are different finished copper weights. Call outs are typically: 1oz, 2oz finished copper or 1oz finished copper on internal layers and 2oz outside layers. Being specific can reduce time in engineering and mistakes in production.
  5. Surface Finish- this seems to be the most forgotten of all the specifications. The dominant surface finish of the past was HASL or Hot Air Solder Level. Bob touched on choosing surface finishes in an early blog post. You should designate: HASL, Lead Free HASL (LF-HASL), Electroless Nickel Immersion Gold (ENIG), Immersion Silver, etc.
  6. Overall Thickness – This is critical for CAM engineers to compare the stack-up in the FAB drawing and draw conclusions about what a customer wants as an overall thickness. The most common overall thickness of a PCB is .062” – other variations are .031”, .093” and there are other custom and specific thicknesses based on a unique stack-up.
  7. Soldermask Color- this is an obvious specification and it should be noted that many factories carry more than just the standard green soldermask that has been so common in the industry. We have had customers order purple, red, blue, etc…keep in mind if you have a specific type of Soldermask requirement that it should be called out in the drawing but most IPC-600 or IPC6012 requirements cover basic soldermask standards.
  8. Legend Color – Same situation as with Soldermask color. There are other legend or silkscreen colors such as yellow, black, etc. most engineers usually include the legend color in their drawings.
  9. PCB Dimensions- This factor really helps a CAM in PCB manufacturing to compare a fabrication drawing with the Gerbers. Most off-shore factories go by the Gerber as the ruling document but we instruct and push our factories to go by the FAB drawing as the ruling document. If there are discrepancies or mistakes with PCB dimensions, it is usually caught in the comparison of the Gerber and FAB drawing.
  10. Array Dimensions & Details – it is very helpful if an OEM does their own production to add the array dimensions, which include but are not limited to: rail size, how many rails and where they want fiducials, mouse bites and other assembly details. Typically EMS companies have their own guidelines and we help design an array that is approved by a production engineer. Make sure to note where you want the fiducials and tooling holes as well.
  11. Controlled Impedance if required – Most engineers who implement CI into their boards typically know what to add to a FAB drawing. Key ingredients are the Ohm figures, coupon details, trace values, etc.
  12. Part Number and Revision with Gerber and FAB drawing being on the same Rev number – it will help your fabricator and EMS company immensely to follow the pattern of having their Gerber file and fabrication drawing at the same revision level. For instance – PN 15-250-01 Rev A should be Rev A for both the Gerber and the FAB drawing and noted changes in the engineering block. There is a lot of potential confusion when the Gerber is Rev A and the fabrication drawing is Rev B.
  13. IPC Specifications
    1. One might add: “All boards to be built to Standard IPC-600 for rigid circuits or IPC-6012 for flex circuits (Latest released revision).”
    2. Class II, Class III
  14. UL Logo – Most all electronic products these days require the UL logo from the PCB Fabricator to be on the PCB somewhere. It can be inconspicuously placed but you should have instructions on the PCB drawing about 1) that you want it on the PCB and 2) how and where you want it placed. A typical note might say: “A UL registered logo is required on all boards.”
  15. Date Code markings – it is wise to point out where you want the date code markings as well. Usually our suppliers put them next to the their UL logo and more often than not always include the date code.
  16. Other Common Notes:
    1. No Ink on Pads
    2. Special Drill Tolerances – most are covered by general IPC specifications but if need to be noted if an engineer has specific requirements outside of general standards.
    3. Drill Hole Charts – these are excellent specifications when placed on a fabrication drawing so the CAM engineer can reference the drawing with the Gerber files and point out any discrepencies.
    4. E-test Requirements – while PCB Solutions requires EVERY flex, rigid-flex or rigid printed circuit board to be tested, some factories may not always make the assumption that you want your product tested…especially if it is easy circuitry in low volumes. That can be missed in the quoting phase if not called out in the drawing.
    5. Other tolerances- Bow & Twist, Aspect Ratio, Surface Finish Thickness, Surface Finish, Silk Screen Registration, Packaging, etc…
  17. Gerber File notations – it is nice, but not always required, to have a FAB drawing that outlines where the artwork and drill data are located with their corresponding file names. Let’s just make it easy on a CAM engineer while we are at it.
With all of that being said, here is an example of a fabrication drawing we see often. It might be too much since a lot of the specifications are covered in the IPC standards but there are also situation where your product needs emphasis…in that case, here is a lot of it.
FABRICATION NOTES: UNLESS OTHERWISE SPECIFIED OR PRE-APROVED
  1. DIMENSIONS AND TOLERANCE:
    1. INCH DIMENSIONS (IN) ARE THE CONTROLLING DIMENSIONS FOR THE DRAWING(S) AND SUPPLIED DATA
    2. DIMENSIONS AND TOLERANCES ARE PER ASME Y14.5M-(LATEST YEAR).
    3. .XX = +/- 0.02 .XXX = +/- 0.005.
    4. WARP AND TWIST OF PCB SHALL NOT EXCEED 1%.
    5. CONDUCTOR WIDTHS AND SPACING SHALL BE WITHIN 20% OR +/- .001 (WHICHEVER IS GREATER) OF ORIGINAL GERBER DATA.
    6. ALL HOLES SHALL BE LOCATED WITHIN +/- 0.003 OR 0.010 DIAMETER OF TRUE POSITION.
    7. LAYER-TO-LAYER REGISTRATION SHALL BE WITHIN 0.005.
    8. SURFACE MOUNT PAD PLATING MUST BE FLAT AND TO A MAXIMUM OF +0.003 ABOVE THE BOARD SURFACE(S).
    9. SILKSCREEN REGISTRATION SHALL BE WITHIN +/- 0.003.
    10. FINISHED THICKNESS INCLUDES SOLDER-MASK.
  2. FABRICATION
    1. FABRICATE PCB IN ACCORDANCE WITH IPC-6012 (CURRENT REVISION), TYPE 3, CLASS 2, PER IPC-6011 (CURRENT REVISION) USING THE DATA FILES SUPPLIED.
    2. FINISHED PCB THICKNESS = 0.062 +/- 10%
    3. REMOVE ALL BURRS AND BREAK SHARP EDGES 0.015 MAXIMUM.
    4. 0.0465 MAXIMUM RADIUS ON ANY INSIDE CORNER(S).
    5. ALL HOLE DIAMETERS ARE REFERENCED AFTER PLATING.
    6. THEIVING IS ALLOWED AS REQUIRED EXCEPT IN PLANE FREE AREAS. COMPANY XYZ IS TO BE NOTIFIED AS TO LOCATIONS ADDED.
    7. ORIGINAL ARTWORK AND/OR FILM (IF SUPPLIED) TO BE RETURNED WITH THE FIRST COMPLETED ORDER.
  3. MATERIAL
    1. PCB SHALL MEET THE REQUIREMENTS OF UL508 AND/OR UL1604 HAZ LOC (IF REQUIRED) WITH A FLAMMABILITY RAILING OR 94V-0 MAXIMUM PCB OPERATING TEMPERATURE SHALL BE NO LESS THAN 140 DEGREE C.
    2. LAMINATE SHALL BE PER IPC-221 PAR 4.2; IN ACCORDANCE WITH IPC-4101/24 (OR BETTER) , PREPPING (B-STAGE) FLAME RESISTANCE MEETING UL 94V-0 GLASS TRANSITION (TG) RATING FOR ALL MATERIAL USED: 140 DEGREE C (MIN) TO 220 DEGREE C ACCEPTABLE.
    3. FINISHED COPPER WEIGHT SHALL BE
  • OUTER LAYERS = 1.5 OZ
  • INTERNAL LAYERS = 1 OZ
  • PLANE LAYERS = 1 OZ
  • HOLES = 0.001 AVERAGE WITH 0.0008 MINIMUM
    • MANUFACURER’S NAME AND/OR IDENTIFICATION
    • Company XYZ PART NUMBER AND REVISION TO WHICH IT WAS MANUFACTURED
    • PURCHASE ORDER NUMBER
    • MANUFACTURED DATE
    • QUANTITY
  1. FINISH
    1. ALL EXPOSED CONDUCTIVE PATTERN AREA(S) NOT COVERED WITH SOLDER-MASK OR OTHER PLATING SHALL BE HOT AIR SOLDER LEVELED (HASL) USING SN63A TIN LEAD SOLDER (OR EQUIVALENT) PER ANSI / J – STD – 006
    2. APPLY LIQUID PHOTO IMAGEABLE (LPI) SOLDER-MASK PER IPC-SM-840, CLASS T, (COLOR; TRANSPARENT GREEN) TO BOTH SIDES OF THE PCB OVER BARE COPPER VIA HOLES COVERED WITH SOLDER-MASK. DO NOT NEED TO BE PLUGGED ONLY SOLDER-MASK IMAGES THAT ARE THE SAME SIZE AS THE COMPONENT PADS MAY BE ENLARGED, AND SHALL NOT BE ENLARGED BEYOND 0.003 PER SIDE. ALL OTHER SOLDER-MASK IMAGES SHALL NOT BE ENLARGED.
    3. SILKSCREEN SHALL BE WHITE, PERMANENT, ORGANIC, NON-CONDUCTIVE INK. THERE SHALL BE NO SILKSCREEN ON ANY SOLDERABLE COMPONENT OR HOLE.
  2. MARKING
    1. Company XYZ: PCB PART NUMBER IS RENDERED IN SILKSCREEN ON THE SECONDARY SIDE OF THE PCB DESIGN. PART NUMBER SHALL BE IDENTICAL TO THIS DOCUMENT AND PURCHASE ORDER.
    2. MANUFACTURER: ‘ORIGINAL’ MANUFACTURER’S UL IDENTIFICATION (LOGO AND/OR FILE NUMBER) 94V RATING, IPC 4101 AND SLASH DESIGNATION, DATE CODE, AND COUNTRY OF ORIGIN SHALL BE RENDERED IN SILKSCREEN INK ON THE SECONDARY SIDE OF THE PCB. LOCATION MAY BE DETERMINED BY THE MANUFACTURER SO LONG AS IT DOEWS NOT ALTER OR OBSTRUCT ANY CURRENT INFORMATION.
  3. TEST REQUIREMENTS:
    1. 100% NETLIST ELECTRICAL VERIFICATION USING SUPPLIED NETLIST FOR OPENS AND SHORTS ALL NETS SHALL BE ACCESS SIMUTANEOUSLY OR AS OTHERWISE MUTUALLY AGREED UPON.
    2. 500VDC HIPOT TEST REQUIRED ON ALL BURIED CAPCITANCE IMAGES AFTER ETCH FINAL 500VDC HIPOT TEST REQUIRE PRIOR TO PACKAGING.
  4. INSPECTION
    1. INPECT PER IPC-600 (CURRENT REV).
  5. REPAIR
    1. PCB REPAIR ACCEPTABLE PER IPC R-700 (CURRENT REVISION).
  6. PACKAGING
    1. COMPLETED PCB’S ARE TO BE QUANTITY SHRINK-WRAPPED AND PACKAGED SUITABLE FOR TRANSIT AND INSPECTION.
    2. EACH QUANTITY WRAP IS TO BE IDENTIFIED (MARKING OR LABEL) PER THE FOLLOWING:
      • MANUFACURER’S NAME AND/OR IDENTIFICATION
      • Company XYZ PART NUMBER AND REVISION TO WHICH IT WAS MANUFACTURED
      • PURCHASE ORDER NUMBER
      • MANUFACTURED DATE
      • QUANTITY
285 likes
Statement: This post is only the personal view of the author and does not represent the opinions of ALLPCB.com.

CurveAudioDesign

Leave A Message

Follow

Impressive
ThreadReply