This page is dedicated to analyzing how to keep costs low by Designing For Manufacturing (DFM). To see the steps involved in PCB manufacturing click [http://www.sunstone.com/pcb-products/pcb-manufacturing-tutorial here.] === Definitions * Annular Rings * The donut ("annulus") created when your drill pierces a copper layer. It is defined as the radius of this donut. For example, a .030" pad with an .020" hole would have a .005" annular ring * Finished Hole Size (Plated Through Holes) * Size of through hole AFTER plating * Plated all the way through the board * Plated Through Holes are normally drilled 4-6 mils over nominal finished hole size. Copper and solder plating generally reduces hole diameter by ~3-5 mils * Unfinished Hole Size (Non-Plated Through Holes) * Size of through hole directly after drilling, BEFORE plating * Aspect Ratio * Board thickness divided by smallest drilled hole (via's). * HIGHER aspect ratios (bigger board thickness, smaller hole) increases probability for voids in holes. * Further Understanding of terminology with '''pictures''' * Sunstone Circuits has a great page [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities here] that has fantastic pictures illustrating what is what in terms of lingo. ---- == Specs to Minimize Fabrication and Assembly Costs == '''Note:''' This list is very conservative, and if followed you should be able to send your design to any manufacturer, assembly house, etc. and get their lowest price possible. === PCB Shape * '''PCB’s must have 2 parallel sides (preferably the 2 longest sides)''' for process through most automated assembly equipment. * Breakaway rails and/or panelization can be used to accommodate a wide variety of odd board shapes. === Board Layer Count & Construction * '''Even number of layers.''' * Odd number of layers lead to warpage problems. * Layer stackup should be symmetrical with regard to dielectrics, copper weights, and layer design. Asymmetrical designs are a primary cause of warped boards. === Copper Weights / Trace Widths / Trace Spacings * Trace line/spacing * '''7/7 mils minimum''' * This is for most common copper weights, like .5oz, 1oz,2oz. For higher weights you will need larger width/spacing. * Copper Weights * '''less CU weight is cheapest.''' Such as .5oz for inner layers and 1oz for outer layers *Go as light as possible and still have good current handeling. === Drill http://www.atechcircuit.com/pcb-capability/rigid-pcb * Hole Size* * Annular Rings * '''For cheapest price across all companies, go >=15mils''' if you can. This includes vias. * Annular Rings * '''7mil minimum''' * Aspect Ratio * '''No higher than 6:1''' * Hole Tolerances * Plated Through Holes * 6 mil window is ideal (+/- 3 mils) * If PTHs over 100 mils are located at the edges of the board, they should have large outer layer pads to prevent too fast plating. * '''Pads 200 mils larger than the hole''' * Non-Plated Through Holes * 4 mil window ---- == Select PCB Fabricator Requirements and Minimums == === OSH Park (Only Fab, no Assembly) * Design Rules * 2 Layer Board Minimums: * Trace Width and Spacing * 6 mils * Traces to Edge of Board * 15 mils * Drill size * 13 mils * Anular Ring * 7 mils * 4 Layer Board Minimums: * Trace Width and Spacing * 5 mils * Traces to Edge of Board * 15 mils * Drill size * 10 mils * Anular Ring * 4 mils * 1.6mm thick (0.063") * 1oz copper on outer layers, 0.5oz on inner layers * Can have internal cutouts (draw on board outline layer) * NO plated slots * Prices and Turnaround times * For prototyping (price includes 3 boards) * 2 Layer boards: $5/square inch. Ship in under 12 calendar days from order * '''NOTE:''' You can get turn time to 5 business days for extra cost of $89 per design. Super Swift Service * 4 Layer boards: $10/square inch. They go to the Fab once a week and have a 2 week turn time once in fab. * Larger orders: * Minimum of 150 square inches (no upper limit) * You can have different designs, but each design must be ordered in multiples of 10 (and in total add up to 150 square inches) * 2 Layers * $1/square inch * Ship in ~3 weeks from order * 4 Layers * $2/square inch * Ship in ~1 month === Advanced Circuits / 4PCB (Fab and Assembly) * Phone Number, sales department in East Cost: 1-800-979-4722 EX. 1339 (Ashley) * Design Rules * All board minimums * Trace Width and Spacing * '''A premium is charged for trace width/spacing less than 7 mils''' * 0.5oz CU (inner layers): 4 mils * 1oz CU (outer layers): 4 mils * 1oz CU (inner layers): 5 mils * 2oz CU (inner & outer): 6 mils * 3oz CU (inner & outer): 10 mils * 4oz CU (inner & outer): 12 mils * Copper to Edge of Board * Outer Layers: 10mils * Inner Layers: 15mils (20 mils preferred) * For Scoring, Outer Layers=15mils Inner Layers=20mils * Drill size * 13 mils * Pad Size/Anular Ring * Vias: * Pad Size=10mils over finished hole size, so annular ring=5mils * Component Holes: * Pad Size=14mils over finished hole size, so annular ring=7mils * Inner Layer Clearances * 10mils * Hole Tolarances * 4mils (if we don't specify, default hole tolerance is 5mils) * Board Thickness (tolerance may vary 10% (min. +/-5mils)) * 2 Layer: 20mils * 4 Layer: 20mils * 6 Layer: 31mils * 8 Layer: 47mils * 10 Layer: 62mils * Rout (board outline and internal cutouts) * +/-10mil tolerances * Slot Width * 31mils * Silkscreen (Legend) * 5mils line width * Offer 0.5,1,2,3,4 oz copper on inner layers, and 1,2,3,4 oz copper on outer layers * NO custom oz CU (like 1.5 or 2.5oz) * Links: * [http://www.4pcb.com/pcb-design-specifications/ Design Specs on website] * Standard Specs: * Non-plated slots & cutouts * Green soldermask, white legend, FR4 * 1oz CU inner layers, up to 2oz CU on outer layers. * Overall thickness: 31,62,93, or 125 mils * Trace/Space at 5/5mils *Gold finders, lead-free solder * Rout Tolerance +/-10mils, Hole Tolerance +/-5mils * Minimum Hole Size=10mils * Fiducials and/or Tooling Holes * Assembly Considerations * PCB Fab MUST be done by 4PCB to have assembly here * [attachment:Advanced-Circuits-Assembly-Requirements.doc Assembly Requirments] * Prices and Turnaround times, fab and assembly * [http://www.4pcb.com/pcb-cam-based-quoting/index.html DFM Check], which will give insight onto clearances that the manufactuer uses * For prototyping: * 2-Layer PCBs * $33 offer * $33/board, minimum of 4 boards '''Note: with Student Program, no minimum PCB quantity. type word 'Student' in COMMENTS section when placing each board. Must have University shipping addresss''' * Turn around time=5 days * Plated or non-plated holes * NO slots, internal routing (cutouts), scoring, tab rout, or drilled hole board seperations. * Minimum 6mils line/space, Minimum 15mil hole size * FR-4, 62mils, 1oz CU * Max size=60in square * Max 35 holes/sq. inch * BareBones * FR-4, 62mils, 1oz CU * Plated or non-plated holes * 6mil line/spacing minimum * Tin finish over 1oz CU * NO internal routing (cutouts), scoring, tab rout, or drilled hole board seperations, mask, legend * Rectangle only * Minimum size: 1.25" x 1.25" Maximum Size: 12" x 16" * Gerber 274X prefered (274D also good) * English Units for drill (Excellon) * Minimum Hole size: 15mils * Max size=60in square * 4-Layer PCBs * $66/board, minimum of 4 boards '''Note: with Student Program, no minimum PCB quantity. type word 'Student' in COMMENTS section when placing each board. Must have University shipping addresss''' * Turn around time=5 days * NO slots, internal routing (cutouts), scoring, tab rout, or drilled hole board seperations. * Minimum 6mils line/space, Minimum 15mil hole size * FR-4, 62mils, 1oz CU * Max size=30in square * Max 35 holes/sq. inch * Larger orders: * Standard Specs are same as above listed. * Custom Specs will cost more. * Fabrication Quotes: *[https://www.my4pcb.com/Net35/Quote/Quote_Code.aspx Quote matrix here.] * Need to know smallest hole size, # pads on top/bottom, thickness, etc * Max quote of 100 boards, larger you need to call *[https://www.my4pcb.com/net35/FreeDFMNet/FreeDFMHome.aspx#_ga=1.239944704.2020970432.1424274393 FreeDFM quote.] * Need gerber files and quote will be emailed to you in minutes. * Also shows potential issues with manufacturing * Talk to a person * Assembly Quotes: * Email the following to a sales rep: * [http://ohm.bu.edu/trac/edf/attachment/wiki/DFM/Assembly-Quote-Checklist.xls Assembly Quote Checklist] * BOM. Here is a [attachment: Assembly-Sample-BOM.xls sample BOM] * CPL (component placement list) or PNP (pick & place file). Here is a [attachment: Assembly-Sample-CPL.xls sample CPL] === Sunstone Circuits (Screamiung Circuits for Assembly) * Design Rules * Depend on service, see below for details * Prices and Turnaround times * Detailed list for all options can be found [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities here.] * '''PCBExpress Quickturn''' and '''''ValueProto PCB Prototype Services''''' * '''Quantity: 1-100''', practically only for small runs 1-15 * Lead times: * PCBExpress Quickturn: * Next Day (2-layer) , 2-Day (2,4-layers), 3-Day (2,4,6-layers) * [http://www.sunstone.com/pcb-products/pcbexpress-quickturn/pcb-quickturn-pricing Pricing] in table form, no input required * Value ProtoPCB: * 5-Days (2-layer) * [https://quoting.sunstone.com/quotevalueproto.aspx Pricing], need demensional input and quantity * '''MUCH cheaper than Quickturn on most orders''' * # of Layers: *1(treated as 2 layer)-6 * Copper Weights: * Inner: 1oz * Outer: 1oz * Trace/Space minimums: * Inner: 6/6mils * Outer: 6/6mils * Clearance for TH drill * Inner: 25mils larger than finished hole size * Pads for TH drill * Inner: 18mils larger than finished hole size * Board Thickness Availible * 62mils ONLY * Soldermask color * Green * Soldermask minimum web (smallest strip possible, such as between two pads NOT INCLUDING soldermask relief) * 5mils * Silkscreen info * [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities#silkscreen Details] * Drill info * 13.5 mils = smallest drill * ValueProto has 23 pre-determined drill sizes [http://www.sunstone.com/pcb-products/pcbexpress-quickturn/file-drill-summary Sizes availible] * [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities#drill More details] * '''Note:''' holes 18mils or less may be plugged * Board Size: * Max: 12" x 14" * Min: .25" x .25" * Slots, Cutouts, Routing, etc: For percise details go to [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities here], and scroll down to Route (Tab) and V-scoring. * Tin-lead finish only * FR-4 * PCBpro Full Feature * '''Quantity: 1-15,000''' * Lead times: * 2 days to 5 weeks * # of Layers: * 1-14 layers * Copper Weights: * Inner: .5, 1, 2oz CU * Outer: 1, 1.5, 2.5oz CU * Trace/Space minimums: * Inner: .5oz CU (5/5mils), 1oz CU (6/6mils), 2oz CU (8/8mils) * Outer: 1oz CU (5/5mils), 1.5oz CU (10/10mils), 2.5oz CU (13/13mils) * Clearance for TH drill * Inner: 20mils larger than finished hole size * Pads for TH drill * Inner: 18mils larger than finished hole size * Board Thickness Availible * 31, 47, 62, 93, 125 mils (and custom thickness) * Soldermask color * green/blue/black/red/white * Soldermask minimum web (smallest strip possible, such as between two pads NOT INCLUDING soldermask relief) * 4mils * Silkscreen info * [http://www.sunstone.com/pcb-capabilities/pcb-manufacturing-capabilities#silkscreen Details] * Drill info * 10mils = smallest drill * [http://www.sunstone.com/pcb-caphttp://www.atechcircuit.com/pcb-capability/rigid-pcbabilities/pcb-manufacturing-capabilities#drill Details] * '''Note:''' holes 18mils or less may be plugged * Board Size: * Max: 14" x 18" * Min: .25" x .25" * Slots, Cutouts, Routing all YES * FR-4 Tg, High Tg, High Td, Low CTE * Fabrication Quotes: * [https://quoting.sunstone.com/dfm.aspx DFMplus quote.] * Need gerber files and quote will be emailed to you in 2 hours. * Also shows potential issues with manufacturing * Easy online quote, no gerber files or specific # of pads required. [http://quoting.sunstone.com/QuoteExpress.aspx Quotes are here] * Talk to a person * Assembly Quotes: * What they need (look [http://www.sunstone.com/pcb-products/assembly-services/file-requirements here] for specifics on the below): * BOM * Gerber Files (RS-274X - same as PCB fabrication) * Centroid (Pick and Place, CPL, and other names). * '''They can generate this from Gerber for an extra charge''' * ASCII-Formateed CAD data * '''ONLY for Short-Run Production Orders''' * Assembly Drawings, instructions or photos * NOT REQUIRED, but "Do help to ensure all special PCB assembly instructions are carried out properly. If requresting any non-standard processes or have ambiguous placements, provide helpful documentation. === Gold Phoenix PCB (Fab and Assembly) *Design Rules * Layers * 1-12 Layers of FR-4 * Minimum Board Thickness * * Prices and Turnaround times *For Quick Online Quote: * wiki:3Dprinting