General data requirementsData for PCB production documentation provided by customers must meet certain criteria in order to make their processing efficient and therefore cheap.
Data formatCAM department processes the customers’ data in Genesis LT software and therefore prefers the ODB++ data format. This data format preserves the attributes from design software and thus prevent errors like mirror layers or wrong inner layers order setup.
|Prefered data format:||ODB++|
|Rest of commonly processed data formats:||Gerber RS-274X|
|*.brd (Eagl version required)|
|Gerber-274D with D-codes list|
|Data formats processed after individual consultation:||DXF|
|Data formats for drilling:||Excellon|
|Sieb & Meyer 1000/3000|
|Gerber RS-274X format layer can be used for drilling where pads represent a diametter of final holes (vias). (recommended)|
Attention! The drilled via diameter is reduced approximately by 1 mm after copper coating due to metal segmentation in the holes. Therefore it´s crucial to specify if a drill diameters or diameters of final vias are mentioned in the customer’s order. If there is none specification mentioned in the order, PCB producer automatically assumes the mentioned diameters as final (after copper coating).
|Suggestion||Gatema - standard CAM processor Eagle|
At DPS processing in Eagle program we recommend to export the data to Gerber RS-274X.
Since the layers are imported by scripts, we recommend to follow still the same layer labels,
which can be implemented to software for following orders.
for optimal labelling and layers export!
|Layer no.||Layer type|
|1, 17, 18||TOP|
|16, 17, 18||BOTTOM|
|29||Top solder mask|
|30||Bottom solder mask|
|21, 25||Top silkscreen|
|22, 26||Bottom silkscreen|
|20||outline / milling|
• If there is no text in the signal layers, we assume that the component (Top) layer is imported correctly.
• Software version, in which the design is made, must be mentioned (example: 6.5.0)!
|PCB outline||Suggested||Not recommended|
|Signal layers||In separate layer||In signal layers|
|line thickness 0,20mm||Line thickness 0,0mm|
|layer label *dim.ger|
|readable text in TOP layer||data without texts|
|one layer = single file||all layers in single file|
|continuous copper in spilled ground||hatched ground|
|deposed, without mirroring, same zero point||scattered|
|min. not plated-through holes isolation gap of 0,20mm pict1||<0,20mm|
|min. buried vias isolation gap of 0,25mm pict2||<0,20mm|
|min. final via lining 0,15mm pict3||<0,15mm|
|data don´t contain zero values|
|copper distance 0,15mm from the PCB´s edge for milling||<0,15mm|
|copper distance 0,50mm from the PCB´s edge for routing||<0,50mm|
|don´t design pads by line|
|Solder mask||min. pads side overlay of 0,10mm pict4||1:1 with motif|
|min. bridge between pads 0,10mm pict5|
|Drilling||min. plated-through hole of 0,15mm||<0,15mm|
|min. blind via of 0,10mm||<0,10mm|
|plated-through hole = copper from both sides||copper from one side = not plated-through hole|
|Milling||Standard diameter of milling device 2,0mm i.e. radius 1,0mm||Tool <0,60mm|
|line thickness 0,18mm||< 0,15mm|
|shapes drawn by polygon|
Data needs to be provided as a single-counted motive. Following panelization is provided by Gatema. If however the final size of multi-count PCB is important, dimensions and tolerance must be provided, possibly with width of technological surroundings, fiduciary marks or other (drawing, panel file, order).