A_Card Design Details ---------------------------- Original Rev. 8-MAY-1997 Most Recent Rev. 16-MAY-1997 Mentor Layer Usage ------------------ Physical Logical Function -------- -------------- -------------------- 1 Signal_1, Pad_1 Component Side 2 Power_1 VCC and cut-lines 3 Power_2 +5V 4 Power_3 +6V 5 Power_4 GROUND and cut-lines 6 Power_5 VTT and cut-lines 7 Power_6 VEE 8 Power_7 -5V 9 Signal_1, Pad_1 Solder Side DAM_1 "Target Area Lable" for Board Outline Artwork Order ------------- Artwork Order Number Layers Special Stuff ------- ---------------------------------- ----------------------------- 1 Board_Outline,Target,Dam_1 2 Signal_1,Pad_1,Target 3 Pow_4,Target Thermal_Relief, Clear 10 mil 4 Pow_1,Pow_2,Pow_3,Target Thermal_Relief, Clear 10 mil 5 Pow_5,Pow_6,Pow_7,Target Thermal_Relief, Clear 10 mil 6 Pow_4,Target Thermal_Relief, Clear 10 mil 7 Signal_2,Pad_2,Target 8 Silkscreen_1,Target 9 Silkscreen_2,Target 10 Solder_Mask_1,Target 11 Solder_Mask_2,Target Artwork Order Number 1 is the Test Plot of the Board Outline. It uses the Dam_1 layer to hold the "Label" for this plot that goes in the target text area. This label is kept on a private layer so that it will not show when the Board Outline is implicitly turn on again during the generation of the planes to generate the plane edge relief. Artwork Order Number 4 is the VCC, +5V, and +6V planes Artwork Order Number 5 is the VTT, VEE, and -5V planes Artwork Order Numbers 3 and 6 are identical GND Planes. One must hand edit the "target area label" between the plots of these two copies of the GND Plane. Gerber File vs Baord Layer File Name Contents Location in Board Stack -------------- ---------------------------- --------------------------- ArtWork_01.Grb Test plot of board outline ArtWork_02.Grb Component side Traces & Pads Component Side ArtWork_03.Grb GND Plane #1 Comp Side GND Next to Component Side ArtWork_04.Grb VCC, +5V, and +6V Planes Next to Next to Comp Side ArtWork_05.Grb VTT, VEE, and -5V Planes Next to Next to Solder Side ArtWork_06.Grb GND Plane #2 Solder Side GND Next to Solder Side ArtWork_07.Grb Solder side Traces & Pads Solder Side ArtWork_08.Grb Component side Silkscreen On the Component Side ArtWork_09.Grb Solder side Silkscreen On the Solder Side ArtWork_10.Grb Solder Mask Component Side On the Component Side ArtWork_11.Grb Solder Mask Solder Side On the Solder Side Hand Edit the two Solder Mask files to cover up all 33 mil vias. Apertures Used -------------- File Name Apertures Used D-Code -------------- ------------------------------ ArtWork_01.Grb D10 ArtWork_02.Grb 10, 11, 12, 13, 14, 15, 16, 17, 18, 19, 70, 71, 20, 21 ArtWork_03.Grb 10, 19, 22, 23, 24, 25, 26 ArtWork_04.Grb 10, 19, 22, 23, 24, 25, 26 ArtWork_05.Grb 10, 19, 22, 23, 24, 25, 26 ArtWork_06.Grb 10, 19, 22, 23, 24, 25, 26 ArtWork_07.Grb 10, 13, 17, 18, 19, 70, 71, 20, 21, 27 ArtWork_08.Grb 10 ArtWork_09.Grb 10 ArtWork_10.Grb 10, 11, 12, 13, 14, 15, 16, 17, 19, 20, 21 ArtWork_11.Grb 10, 13, 17, 18, 20, 21 By hand edit pull the 33 mil via solder mask off of both Solder Mask files, i.e. file 10 and 11, i.e. pull D20 from these files. Hole Count ---------- Finished Size Count ------------- ------- 13 173 40 417 113 8 By had move from the DIRAC [...A_Card] directory to the /Copy_to_Flop_Dir directory the following files: APERTURE_TABLE_REPORT.TXT ---> aperture.txt DRILL_TABLE_REPORT.TXT ---> drill.txt Manufacture_Instructions.TXT ---> instruct.txt COPY_TO_FLOPPY_DIRECTORY.SH located in /a_card_uber is used to move Gerber and drill data files from /pcb/mfg to the /Copy_to_Flop_Dir