1. RECOMMENDATION: ALWAYS include a Gerber mechanical layer in your data set.
- A proper mechanical layer is VITAL to a good and flawless production of the PCB as it should provide us with all the needed mechanical information for the construction of your PCB.
- In case of cut-outs or slots in your PCB, this layer is essential to the production!
- DO NOT scale your mechanical layer, it should be 1 to 1 and reflect the exact dimensions of the PCB.
- The mechanical layer is – as for all layers - also viewed from top to bottom through your PCB, so do not mirror the mechanical layer.
- ONLY include information in your mechanical layer that is needed
2. Do not provide actual routing layers for board contours or inside milling.
Routing data is production-specific depending on the rout tools, tool compensations, routing order and direction used by each PCB fabricator. This means that we cannot use customer-provided routing layers. We need to completely rework them, which can lead to confusion and misinterpretations which may result in incorrect boards.
It is our job as board producers to prepare correct production routing layers based on the information in your mechanical layer
3. A mechanical layer should MINIMALLY contain:
- The exact board outlines, ideally including dimensions (mm or inch).
- Exact positions and sizes for all inside milling, slots or cutouts, ideally including dimensions (mm or inch).
Outlines are best shown using a small line - e.g. 0.50mm (20mil) wide - where the center of the line represents the exact board outline.
When no dimensions are given we will always take the center of the contour lines to be the exact outline of the board, regardless of their thickness.
4. Additional information that should be included in the mechanical plan when needed:
- A reference hole: the distance from one drill hole in X and Y to the PCB outline. This is particularly important when you only have NPTH holes without copper pads.
- Positional indication of all drills using symbols (=drill map). Use different symbols for each different drill size.
- PTH/NPTH indication for holes and slots
- If you supply panelized data include proper indications for break-routing and/or scoring (V-cut)
- A clear layer sequence or buildup drawing including all copper layers, soldermask and legend layers, any additional layers like peel-off or carbon, in the correct sequence viewed from top to bottom and with the correct corresponding data file name.
- Special build-up: If the build of your PCB requires material thicknesses, copper thicknesses or multilayer buildups which are different from our standard values then add this information to the layer sequence or buildup drawing.
We ONLY use a drill map to cross-check the Excellon drill file(s) for correctness. A drill map will NEVER be used to generate a drill file as this gives too many opportunities for error.
5. The standard tool size used for all outline routing is 2.00mm (79mil).
This means that the standard minimum radius for inside corners is 1.00mm (39.5mil).
Requirements for a smaller radius on inner corners should be clearly indicated in the mechanical layer.
A sharp or 90 degrees inner corner can be obtained by placing a properly sized NPTH drill exactly on the board outline center of the inner corner or by a clever design of your board outline.
6. The smallest width for any routed slot is 0.50mm (20mil) ENDSIZE.
7. Standard mechanical tolerances.
Tolerance on contour dimensions +/- 0.20mm (+/- 8mil) Tolerance on position of contour/cutouts to holes +/- 0.20mm (+/- 8mil) Tolerance on slot dimensions
Width +/-0.10mm (+/- 4mil)
Length +/-0.20mm (+/- 8mil)
Scored (V-cut) boards
Tolerance on contour dimensions (after board separation) +/- 0.30mm (+/- 12mil)
When no tolerances are specified in your data, we will produce according to our standard tolerance specifications.
If you require tighter tolerances these should be clearly indicated in the mechanical layer and tool list. They will increase the cost of the PCB so should not be used without a compelling reason.