PCB manufacture "instructions" Q
in [Design]
|
Prev: Optics
Next: low MHz connector design consultant
From: Robert Baer on 29 Apr 2010 17:46 What other info should be included: 106AC-1d 04-17-2010 [this is name of board and date submitted] Basic Information: 30 Pieces - 8 Day Lead Time 0.8 x 2.3 Inches (2 Inch Mounting Centers) Double Sided PCB Details: TG-170 or Higher FR-4 .062 Board Thickness One Ounce Copper ENIG Finish BOTH Sides BLUE Solder Mask BOTH Sides WHITE Silk Screen BOTH Sides Pads / Holes: Minimum Annular Ring / Restring .012 Number of Pads: 61 Number of Vias: 0 Number of Smds: 2 Smds in Top: 2 Smds in Bot: 0 Number of holes: 0 Blind or Buried Vias: 0 Total number of drills: 61 Gerber RS-274X File Extension Key .cmp - Top Copper / Component Side .sol - Bottom Copper / Solder Side .plc - Top Silk Screen Legend .pls - Bottom Silk Screem Legend .stc - Top Solder Mask Stop .sts - Bottom Solder Mask Stop .dim - Dimensions / PCB Outline .drd - Plated-Thru Drillings (Excellon) .hol - Unplated Drillings (Excellon) *Not Used if Absent* .mill - Milling *Not Used if Absent* .info - Information Files *Disregard if Not Needed* Contact Information: (contact name) (company name) Phone: Telefax: E-mail: Web URL: Shipping or Mailing Address: (contact name) (company name) (company address) (city state zip)
From: Martin Riddle on 29 Apr 2010 18:23 "Robert Baer" <robertbaer(a)localnet.com> wrote in message news:xKOdnd1ePMepY0TWnZ2dnUVZ_qCdnZ2d(a)posted.localnet... > What other info should be included: > > 106AC-1d 04-17-2010 [this is name of board and date submitted] > > Basic Information: > 30 Pieces - 8 Day Lead Time > 0.8 x 2.3 Inches (2 Inch Mounting Centers) > Double Sided > > PCB Details: > TG-170 or Higher FR-4 > .062 Board Thickness > One Ounce Copper > ENIG Finish BOTH Sides > BLUE Solder Mask BOTH Sides > WHITE Silk Screen BOTH Sides > > Pads / Holes: > Minimum Annular Ring / Restring .012 > Number of Pads: 61 > Number of Vias: 0 > Number of Smds: 2 > Smds in Top: 2 > Smds in Bot: 0 > Number of holes: 0 > Blind or Buried Vias: 0 > Total number of drills: 61 > > Gerber RS-274X File Extension Key > .cmp - Top Copper / Component Side > .sol - Bottom Copper / Solder Side > .plc - Top Silk Screen Legend > .pls - Bottom Silk Screem Legend > .stc - Top Solder Mask Stop > .sts - Bottom Solder Mask Stop > .dim - Dimensions / PCB Outline > .drd - Plated-Thru Drillings (Excellon) > .hol - Unplated Drillings (Excellon) *Not Used if Absent* > .mill - Milling *Not Used if Absent* > .info - Information Files *Disregard if Not Needed* > > Contact Information: > (contact name) > (company name) > Phone: > Telefax: > E-mail: > Web URL: > > Shipping or Mailing Address: > (contact name) > (company name) > (company address) > (city state zip) Some notes I use, these are on a drill drawing that has all the drill information. (usually the drill dwg is enough to quote) My gerbers include a txt file with the layer descriptions and contact info of the designer. Notes: 1. MATERIAL 0.062 THICK, EPOXY GLASS FR-4, 1OZ. COPPER CLAD BOTH SIDES BEFORE PLATING. 2. FRONT TO BACK REGISTRATION TO BE WITHIN 0.0025". 3. HOLES NOT DIMENSIONALLY LOCATED SHALL BE WITHIN 0.005" OF THE POSITION AS LOCATED ON THE MASTER DRAWING. 4. UNLESS OTHERWISE SPECIFIED ALL HOLES SHALL BE PLATED-THRU HOLE DIAMETER TOLERANCES APPLY AFTER PLATING. 5. ELECTROPLATED COPPER SHALL BE USED FOR THE PLATED-THRU HOLES, AND SHALL HAVE A MIN. THICKNESS OF 0.001" ON THE HOLE WALLS. 6. ALL EXPOSED CONDUCTIVE SURFACES ON LAYERS 1 AND 6 INCLUDING PLATED-THRU HOLES, SHALL HAVE AN ELECTROPLATED SOLDER COART WITH A MIN. THICKNESS OF 0.0003". THE SOLDER COAT SHALL CONTAIN A MIN. OF 60% TIN. 7. WHERE APPLICABLE, EDGE FINGERS ARE TO BE GOLD PLATED .00005" MIN. OVER NICKEL .00020" MIN. (TO DIMENSION SHOWN) 8. BOARDS SHALL BE SOLDER MASKED ON LAYER 1 AND 6 OVER BARE COPPER CONDUCTORS. THE SOLDER MASK SHALL BE GREEN SOLDER RESIST LIQUID PHOTO-IMAGEABLE, MATTE FINISH. 9. SOLDER MASK SHALL BE APPLIED PRIOR TO SCREENING. 10. SCREEN ALL LEGENDS IN WORNOW INK 50-100, GLOSS WHITE. 11. BOARD MUST BE ETCHED IN COPPER ON SOLDER SIDE WITH MANUFACTURER NAME, INITIALS OR LOGO, UL RECOGNITION MARK AND FLAME RATING IN LOCATION SHOWN. Note 11 is a must for UL products. Cheers
From: Robert Baer on 29 Apr 2010 23:36 Martin Riddle wrote: > "Robert Baer" <robertbaer(a)localnet.com> wrote in message > news:xKOdnd1ePMepY0TWnZ2dnUVZ_qCdnZ2d(a)posted.localnet... >> What other info should be included: >> >> 106AC-1d 04-17-2010 [this is name of board and date submitted] >> >> Basic Information: >> 30 Pieces - 8 Day Lead Time >> 0.8 x 2.3 Inches (2 Inch Mounting Centers) >> Double Sided >> >> PCB Details: >> TG-170 or Higher FR-4 >> .062 Board Thickness >> One Ounce Copper >> ENIG Finish BOTH Sides >> BLUE Solder Mask BOTH Sides >> WHITE Silk Screen BOTH Sides >> >> Pads / Holes: >> Minimum Annular Ring / Restring .012 >> Number of Pads: 61 >> Number of Vias: 0 >> Number of Smds: 2 >> Smds in Top: 2 >> Smds in Bot: 0 >> Number of holes: 0 >> Blind or Buried Vias: 0 >> Total number of drills: 61 >> >> Gerber RS-274X File Extension Key >> .cmp - Top Copper / Component Side >> .sol - Bottom Copper / Solder Side >> .plc - Top Silk Screen Legend >> .pls - Bottom Silk Screem Legend >> .stc - Top Solder Mask Stop >> .sts - Bottom Solder Mask Stop >> .dim - Dimensions / PCB Outline >> .drd - Plated-Thru Drillings (Excellon) >> .hol - Unplated Drillings (Excellon) *Not Used if Absent* >> .mill - Milling *Not Used if Absent* >> .info - Information Files *Disregard if Not Needed* >> >> Contact Information: >> (contact name) >> (company name) >> Phone: >> Telefax: >> E-mail: >> Web URL: >> >> Shipping or Mailing Address: >> (contact name) >> (company name) >> (company address) >> (city state zip) > > Some notes I use, these are on a drill drawing that has all the drill > information. (usually the drill dwg is enough to quote) > My gerbers include a txt file with the layer descriptions and contact > info of the designer. > > Notes: > > 1. MATERIAL 0.062 THICK, EPOXY GLASS FR-4, 1OZ. COPPER CLAD > BOTH SIDES BEFORE PLATING. > > 2. FRONT TO BACK REGISTRATION TO BE WITHIN 0.0025". > > 3. HOLES NOT DIMENSIONALLY LOCATED SHALL BE WITHIN 0.005" > OF THE POSITION AS LOCATED ON THE MASTER DRAWING. > > 4. UNLESS OTHERWISE SPECIFIED ALL HOLES SHALL BE PLATED-THRU > HOLE DIAMETER TOLERANCES APPLY AFTER PLATING. > > 5. ELECTROPLATED COPPER SHALL BE USED FOR THE PLATED-THRU > HOLES, AND SHALL HAVE A MIN. THICKNESS OF 0.001" ON THE > HOLE WALLS. > > 6. ALL EXPOSED CONDUCTIVE SURFACES ON LAYERS 1 AND 6 > INCLUDING PLATED-THRU HOLES, SHALL HAVE AN ELECTROPLATED > SOLDER COART WITH A MIN. THICKNESS OF 0.0003". THE SOLDER COAT > SHALL CONTAIN A MIN. OF 60% TIN. > > 7. WHERE APPLICABLE, EDGE FINGERS ARE TO BE GOLD PLATED > .00005" MIN. OVER NICKEL .00020" MIN. (TO DIMENSION SHOWN) > > 8. BOARDS SHALL BE SOLDER MASKED ON LAYER 1 AND 6 OVER BARE > COPPER CONDUCTORS. THE SOLDER MASK SHALL BE GREEN SOLDER > RESIST LIQUID PHOTO-IMAGEABLE, MATTE FINISH. > > 9. SOLDER MASK SHALL BE APPLIED PRIOR TO SCREENING. > > 10. SCREEN ALL LEGENDS IN WORNOW INK 50-100, GLOSS WHITE. > > 11. BOARD MUST BE ETCHED IN COPPER ON SOLDER SIDE WITH MANUFACTURER > NAME, INITIALS OR LOGO, UL RECOGNITION MARK AND FLAME RATING > IN LOCATION SHOWN. > > > Note 11 is a must for UL products. > > Cheers > > > Thanks. Made some changes before your posting: 106AC-1d Order Information: Date Ordered: April 17, 2010 Number of Pieces: 30 Count Lead Time Requested: 8 Days PCB Identifying Marks: 106AC-1d Units of Measure: Inches / Mils (.001 Inch) PCB Specifications: Size (Each): 0.8 x 2.3 Inches (2 Inch Mounting Centers) Layers: Double Sided Laminate: TG-170 or Higher FR-4 Thickness: .062 / .063 Inch Copper Weight: One Ounce PCB Finish: Finish: ENIG*******BOTH Sides Solder Mask: BLUE LPI***BOTH Sides Silk Screen: WHITE******BOTH Sides Pads / Holes Data: Minimum Annular Ring: .012 Number of Pads: 61 Number of Vias: 0 Number of Smds: 6 Smds in Top: 4 Smds in Bot: 2 Number of Holes (NPTH): 0 Total Number of Drills: 61 Different Drill Sizes: 5 Gerber RS-274X File Extension Key: .cmp - Top Copper / Component Side .sol - Bottom Copper / Solder Side .plc - Top Silk Screen Legend .pls - Bottom Silk Screem Legend .stc - Top Solder Mask Stop .sts - Bottom Solder Mask Stop .dim - Dimensions / PCB Outline .drd - Plated-Thru Drillings (Excellon) .hol - Unplated Drillings (Excellon)****Not Used if Absent .mill - Milling**************************Not Used if Absent .info - Information Files****************Disregard if Not Needed Contact Information: (...) Shipping or Mailing Address: (...)
From: Michael Karas on 30 Apr 2010 00:31 In article <xKOdnd1ePMepY0TWnZ2dnUVZ_qCdnZ2d(a)posted.localnet>, robertbaer(a)localnet.com says... > > Gerber RS-274X File Extension Key > .cmp - Top Copper / Component Side > .sol - Bottom Copper / Solder Side > .plc - Top Silk Screen Legend > .pls - Bottom Silk Screem Legend > .stc - Top Solder Mask Stop > .sts - Bottom Solder Mask Stop > .dim - Dimensions / PCB Outline > .drd - Plated-Thru Drillings (Excellon) > .hol - Unplated Drillings (Excellon) *Not Used if Absent* > .mill - Milling *Not Used if Absent* > .info - Information Files *Disregard if Not Needed* > I would recommend showing a table of all the layers in order from top to bottom so as to make it clear what your stackup order really is. Here is an example: Layer Definitions: Top Paste Artwork: paste_top.pho Top Silk Artwork: silk_top.pho Top Mask Artwork: mask__top.pho Top Side Artwork: art_top.pho Internal Ground Plane: art_gnd.pho Internal Power Plane: art_pwr.pho Bottom Side Artwork: art_bot.pho Bottom Mask Artwork: mask__bot.pho Drill Data File: drilldat.drl (Note layer order is numbered on the artwork layers with layer 1 being the top side layer and layer 4 being the bottom side layer.) If you do not have a fab drawing that shows things like stackup, hole size table, routing/v-grooving details, fab notes, dimensions, multi-packing and others then consider making one of these for each project. Some layout packages make it straight forward to generate the fab drawing as another layer in the CAD tool. I often find it more straightforward to just do the fab drawing in another package such as AutoCad. I find it is actually easier for me to re-use portions of one fab drawing to the next when they are in a separate tool. -- - mkaras
From: Nial Stewart on 30 Apr 2010 06:11
One other thing is permission to remove unconnected pads in internal layers (if you haven't removed these in the gerbers, and you don't mind them being removed). Nial. "Robert Baer" <robertbaer(a)localnet.com> wrote in message news:xKOdnd1ePMepY0TWnZ2dnUVZ_qCdnZ2d(a)posted.localnet... > What other info should be included: > > 106AC-1d 04-17-2010 [this is name of board and date submitted] > > Basic Information: > 30 Pieces - 8 Day Lead Time > 0.8 x 2.3 Inches (2 Inch Mounting Centers) > Double Sided > > PCB Details: > TG-170 or Higher FR-4 > .062 Board Thickness > One Ounce Copper > ENIG Finish BOTH Sides > BLUE Solder Mask BOTH Sides > WHITE Silk Screen BOTH Sides > > Pads / Holes: > Minimum Annular Ring / Restring .012 > Number of Pads: 61 > Number of Vias: 0 > Number of Smds: 2 > Smds in Top: 2 > Smds in Bot: 0 > Number of holes: 0 > Blind or Buried Vias: 0 > Total number of drills: 61 > > Gerber RS-274X File Extension Key > .cmp - Top Copper / Component Side > .sol - Bottom Copper / Solder Side > .plc - Top Silk Screen Legend > .pls - Bottom Silk Screem Legend > .stc - Top Solder Mask Stop > .sts - Bottom Solder Mask Stop > .dim - Dimensions / PCB Outline > .drd - Plated-Thru Drillings (Excellon) > .hol - Unplated Drillings (Excellon) *Not Used if Absent* > .mill - Milling *Not Used if Absent* > .info - Information Files *Disregard if Not Needed* > > Contact Information: > (contact name) > (company name) > Phone: > Telefax: > E-mail: > Web URL: > > Shipping or Mailing Address: > (contact name) > (company name) > (company address) > (city state zip) |