Resources

PCB Design Guidelines

Supported Design File Types:

• Gerber files (RS274-X preferred) including 
  • Excellon Drill Files 
  • Drill Tool List (sometimes embedded in Drill File) 
  • Top and Bottom Copper Layers (positive polarity)
  •  Inner layers (polarity based on design) 
  • Top and Bottom Soldermask (negative polarity - presence of data will represent the absence of soldermask on the board. Outline only will cover the board entirely with soldermask)
  •  Top and Bottom Silkscreen (positive polarity) 
  • Board Outline (if not already present on another layer) 
  • Aperture / D-Code List (if file set is not RD274-X compliant) 
  • Readme file or fabrication drawing with file information to match your uploaded files listing the Gerber layers and the NC drill files in the order they will be built. 
  • Material layer stack up (dielectric thicknesses and copper weight requirements) if requesting a non-standard stack up.
  • Any additional PCB files will be ignored for an Engineering Level = Limited Review order. ​
     
• Native Design Files submitted from: 
  • EAGLE 
  • Altium (Protel) 
  • OrCAD (with .MAX file extension) 
  • Ultiboard (National Instruments' Circuit Design Suite) 
  • IVEX PCB123

 If your needs go beyond our Limited Review Engineering Level capabilities, chose Engineering Level = Full Review (NRE) in the OneQuote form. Your files will undergo a design review by our Pre-engineering team looking for manufacturability and insure that the print notes, PO notes and other files included are read and followed. This will also allow Sunstone to make small edits to the files to improve manufacturability and NRE charges will apply. Positive Polarity - When the elements drawn in the CAD file represent the copper / silk or soldermask features with the polygons (usually colored). i.e if the colored portion of the file layer represents the data portrayed it is considered positive polarity

PCB Drill File Requirements

General Requirements for Drill File Submission

• Must be submitted in Excellon format 
• Must be ASCII text viewable. Please open with "Word" or "notepad" to verify a numeric list of X & Y coordinates. (There should be no strange graphical characters).
• PCB drill files should not contain "G01", "G54" or and reference to "D" codes when opened in a text editor. (This indicates a Gerber format and is most likely a drill drawing rather than an NC file). 
• Properly formatted PCB Drill files have sizes separated with "T" codes that indicate tool numbers. (T01, T02, etc.) 
• A tool report with the drill sizes necessary (if not contained in the drill file header). 
• Include a fab drawing, NC Drill File, or Gerber file for slots and / or cutouts. This file should define the slot or cutout size, shape and location. 
  • To achieve a plated slot or cutout place the feature on the drill layer and include an outerlayer pad at least the size of the slot or cutout to be plated. Maximum diameter for a plated feature is 0.250" 
  • Non-plated slots or cutouts should be placed on the outline layer. There is no limit to the size or shape. 

  • The largest drill size available is a 0.250". All holes >0.250" are considered a cutout as they require additional programming and drill time.

     

 Standard Operating Process: 

• All PCB holes are viewed from the top layer of the board. 

• All holes will be treated as through holes unless specifically indicated otherwise and indicated on the OneQuote order. 

   

Restrictions for LIMITED REVIEW boards:

• No blind or buried vias are supported. 
• Holes marked in the files as non-plated through holes cannot be guaranteed to remain unplated. (removing the copper pad on the top and bottom layer of the hole will provide the best opportunity to achieve non-plated holes). 
• All holes > 0.250" will be non-plated and must be ordered as a cutout to maintain the correct size. 
• Spacing between holes at least 0.012" (edge to edge). Holes that do not meet this requirement will be placed on hold until resolved. 
  • For "perforation holes" between boards Sunstone may remove or decrease diameter to increase the distance between holes. 
• Limit number of holes to less than 50 per square inch. 
• Sunstone cannot create the drill file from a Gerber file, fab document or drawing. Please include an Excellon formatted file. 
• Specified holes < 0.018" will be treated as vias and drilled approximately the same size as specified in the drill file. 
• Smallest drill size available for ValueProto PCBs is a 0.0135". Any holes smaller than 0.0135" will be increased to this size. 
• Slots or cutouts are not available for a ValueProto PCB. 
• Holes that overlap the board edge (castellated holes) cannot be guaranteed to meet IPC standards with a Limited Review selection. The holes may not be centered in the route path, plating may be removed from the barrel during routing and there may be excess copper on the board edges around the drilled holes. If you require conformance to IPC requirement, please select an Full Review (NRE).

Circuit Board Routing Outline

Perimeter PCB Routing Details (Individual) 

Sunstone will program the circuit board routing from the outline of the PCB. The outline must be continuous with overall board dimension calculated from the center of the outline. 

• The standard tolerance for online product for the dimensions is +/- 0.010". 
• Copper backset of 0.020" is recommended to prevent damage of the copper features during the routing process.
•  Round or odd shapes are allowed if the guidelines are followed. 

PCB Routing Restrictions

• Limit of 1 router pass to the outside perimeter of the PCB drawn with a continuous line. 
• Connected or panelized boards (submitted as such in files) will not be cut apart by Sunstone.
  •  Sunstone recommends that you separate these boards that you wish to cut apart by at least 0.100" 
  • Tools such as a Dremel, rotary cutter or small saw work well to cut these boards apart. 
• Breakaway or perforation holes in your design: please maintain at least 0.010" edge to edge spacing between these holes (minimum hole size 0.0135") 
• Inside chamfer are not recommended. (Inside cut made usually at 45º angle to the adjacent edge). If necessary please allow for a 0.093" diameter router (inside radiuses and copper to board edge).

Board Outline

Perimeter PCB Routing Details:

Our process will program the circuit board routing automatically by reading the path of your outline. The outline must be a continuous line. The board dimensions are determined from the center of the line used to draw the outline and will be routed to a +/- 0.010" tolerance. You should leave 0.020" space from the routed edge of the board to the nearest copper feature. 

PCB Routing Restrictions: 

1. Limit to 1 pass of outside board perimeter using a continuous line. 
2. If you are adding your own break away or perf holes, please leave at least 0.010" between holes.
3.  Inside Chamfer or an inside cut made usually at a 45 degree angle to the adjacent edges are not recommended. If necessary to your design, please allow for a 0.093" diameter router on the inside radius.

PCB Order Checklist

This checklist is a tool to help ensure that you have the correct Gerber PCB layout guidelines before submitting your order. 

Gerber PCB File Submission: 

• My files are contained in a single compressed file (.zip) containing only the required files 
• Once my order is put into process no additional changes to the files will be permitted. 

Gerber Layer File Preparation: 

• Preview files in a Gerber viewer prior to submission to insure that the files have exported as you expected.
• Verify that the board design fits into the Sunstone manufacturing Capabilities 
• Gerber files format is either RS274X (embedded apertures) or RS274D (with aperture list separately) 
• All external layers (top and bottom) are positive polarity 
• Files do not require manual merging 
• Power / Ground / mounting holes have sufficient clearance to the copper layers to prevent shorting. 

Single SIded - 1 layer Boards: PLEASE PREVIEW ALL 1-Layer Files 

• Preview files as if viewed looking through the top (component) layer side. 
• Right Reading copper text is drawn on the single side (+silk screen if applicable) 
• Single sided boards (Limited Review - Prototype) will contain plated through holes (pads will be added to the opposite side) 

Multilayer Boards: 

• Internal layers are individual layers (either positive or negative polarity) that do not require merging. 
• Internal ground layers contain sufficient clearances for all holes including non-plated and mounting holes. 
• Ground and Power layers are marked to indicate proper polarity 

Board Outline: 

• Cut shape is drawn around board perimeter using a continuous line. 

Drill Setup: 

• ASCII text file provided showing the X and Y coordinates of the holes.
• My NC drill file is NOT a Gerber layer or drawing. 
• Separate tool size list included or the tool sizes are listed within the header of my Excellon drill file. 

Slot / Cutouts:

• These features are indicated on the outline layer. 
• The minimum width for a plated slot is 0.020" 
• The minimum width for a non-plated slot is 0.031" Solder Mask Top and Bottom (as required) files have been included Solder mask swell is at least 0.008" larger than the copper features to keep solder mask off of copper features. 

Silk Screen: 

• Top and Bottom (as required) files included 
• Silk screen is drawn with a minimum 0.006" aperture line width to ensure legibility. 

Native File Upload: 

• For EAGLE Users: please include a readme with your object layers defined. If these are not documented: 
  • Top silk layer: Sunstone will default to object layer 21 (tplace) and 25 (tnames) 
  • Bottom silk layer: Sunstone will default to object layer 22 (bplace) and 26 (bnames) 
  • All midlayer object layer selections MUST be documented in your file set.