Tolerances 

1. Inner Layer Clearances
   We require a minimum of 0.010" inner layer clearance.
   
   
2. Copper to Edge of Printed Circuit Board
   Minimum of 0.010" (outer layers) and 0.015" for inner layers (0.020" preferred for inner layers). For scoring, minimum of .015 for outer layers and .020 for inner layers.
   
   
3. Pad Size/Annular Ring
   Pad size should be at least + 0.010" over finished hole size for vias and + 0.014" over finished hole size for component holes. This means the annular ring (radius of the pad) should be at least .005" for vias and a minimum of 0.007" for component holes.
   
   
4. Hole Size
   +/- 0.005"  Standard Spec (applies to holes up to .250", larger holes will be routed, see Rout tolerances below)
   +/- 0.005"  Custom Spec
   +/- 0.003" Custom Spec upon request 1 oz and 2 oz finished copper weight only.
   -Minimum finished hole size; 0.010". Call your salesperson if you required a finished hole size less than 0.010".
   -If the hole tolernaces are zero, then Advanced Circuits will asssume that the customer is ok with our default hole tolerance.  Our default hole tolerance listed above.
   
   
   
5. Printed Circuit Board Thickness
   Overall may vary +/- 10% (Minimum +/- 0.005")
   Minimum finished thickness for 2-layer: 0.005" (Call if you need a thickness of less than 0.005")
   Minimum finished thickness for 4-layers: 0.020"
   Minimum finished thickness for 6-layers: 0.031"
   Minimum finished thickness for 8-layers: 0.047"
   Minimum finished thickness for 10-layers: 0.062"
   
   
6. Inner Layer Thickness
   Tolerances do not apply to the inner layers of prototypes.
   
   
7. Rout (Board Outline and Internal Cutouts) 
   The Outer Layer Tolerances on Standard Spec defined boards is +/- 0.010" 
   (+/- 0.005" available for Custom Spec upon request)
   Note: We rout to your board size using the center of the board outline on your mask layer.
   
   
8. Copper Trace Width/Spacing
   This is the minimum air gap between any two adjacent copper features. Trace width is the minimum width of a copper feature, usually traces.
   For trace width/spacing, we require a minimum of 0.005" for 1 oz. finished copper weight on outer layers. Premiums are added for trace/space specs less than 0.008"
   For 1 oz. finished copper weight (inner layers), minimum trace width/space is 0.005"
   For 2 oz. finished copper weight (inner & outer), minimum trace width/space is 0.006"
   For 3 oz. finished copper weight (inner & outer), minimum trace width/space is 0.010"
   For 4 oz. f inished copper weight (inner & outer), minimum trace width/space is 0.012"
   
   
9. Trace Width/Air Gap
   The greater of +/- 20% or +/- 0.002"
   
   
10. Soldermask Swell
    This is the expansion of mask relief over pad area. Our minimum is 0.005" over pad dimension or 0.0025" each side. Advanced Circuits will modify files to meet the minimum dimension.
    
    
11. Slot Width
    Minimum 0.031" in width. For smaller width, call your salesperson for pricing and turntime.
    
    
12. Tab Rout Spacing
    Please allow 0.100" spacing between your individual pcbs for tab rout spacing. When scoring there should be no spacing between boards.
    
    
13. Silkscreen (Legend)
    0.005" minimum line width.