Our production site will be closed for the Christmas holidays from 24 December 2018 to 04 January 2019 inclusive.

Solder Resist Mask

1. Due to alignment process the soldermask clearances over copper pads must be compensated for the pcb production according to the fact that in any case the copper pads must be not covered by solder resist material more than 0.25um(1mil) – cfr IPC A600. So it is suggested to oversize those clearances. If the oversizing will be not present in the gerber files or it is not enough for the production some change could be set during CAD/CAM operations respecting the PCBOARDS Classes table which indicates the minimum values.

2. Soldermask clearances rules are followed during CAD/CAM operation to change the solder mask layers if the gerber file is not correctly realized (so if the mask clearances are not oversized enough for the production). The rules are thought considering that the clearances compensation is set according to the PCB pattern class. The different features are:

- depending on pcb class the mask clearance’s dimension could be ugual to the same location copper pads more 250um: also lower values of increment are possible as they were indicated in related table.
- the minimum line of solder resist material ( gap between different clearances) will be not less than 100um ( 4mil) for green colour of resist; for minimum values related to different resist colours see related table.

- the minimum distance between a mask clearance and a copper line ( track, grid or full plane) will be not less than 100um ( for minimum value see related table)

- the minimum distance between a mask clearance (on a SMD pad) and a PTH or via hole (connected to the same SMD pad) must be not lower than 0.15mm ( 6mil). If not respected during assembling process solder paste printed on that SMD pad could flow into the hole reducing the solder joint.

Normally the CAD/CAM process applys the general values to the complete soldermask; then, depending on the design, some clearances could be reduced at particular places down to the minimum accepted values to generate the best soldermask.

Important note: solder dum ( mask segments) smaller then 89um (3.5mil) will be removed; this means that multiple clearances, even if oversized at the minimum value, with gap between them lower than 89um, will be realized as one only mask clearance ( clearance totally opened over multiple Cu pads).

3. On Npth’s (with no Cu pads) or slot’s position, a mask clearance of 125um (5mil) will be always put independently from the pcb class.

4. Hole covering is not guarantee even if no any clearance is generate on the soldermask layer (gerber file): this means that even if the via holes or PTH will be covered by solder resist material, the holes will not be fully closed or covered by that.

Important note: a Plug-in process or Viafilling process will be needed to get vias or PTH fully closed or covered by solder resist material; this must be clearly indicated in the soldermask layer ( file gerber) and it is allowed only for PcbOnDemand service.

5. The board outline should be included in the soldermask layers ( as usual for other layers – mechanical or copper): if a small area of the pcb’s edge must be free of solder resist material this must be clearly indicate on the soldermask layers or on the mechanical layer.

6. Also some peelable solder resist material could be put on the pcb if required (only for PcbOnDemand service); this special material is normally used to protect defined holes or pads against mass soldering. It is also used to protect gold-plated contacts or carbon elements during same process. After soldering process it will be removed (peeled away from the pcb) to finish the assembling process of the boards. The peelable material is not photoimageable so the printing process is the screen printing: for this reason the alignment/registration tolerance are +/-0.4mm (+/-16mil).

Some rules must be followed to get the correct result of this special material:
- peelable should be put only on 1 side of the pcb.
- the board outline presence in the peelable layer is mandatory to put it in correct position on the pcb.
- the minimum width of any peelable line is 1mm (40mil) in one direction and 5mm (200mil) in the other; so minimum peelable area must be 5mm2. Nevertheless it is suggested to use not any line thinner than 3mm (120mil), because thinner line are easy to remove during handling of pcb and/or hard to remove after solder processes.
- holes with diameter bigger than 3mm (120mil) will be covered only over their copper anular ring: the complete filling with peelable material is not guaranteed for these sizes of hole ( so it is possible that they will be not totally closed).
- the correct thickness of the peelable material si not lower than 0.2mm and not higher then 0.7mm.
- due to alignment/registration tolerance of the peelable and its slump during printing process:
# the minimum distance from peelable area to free copper is 0.6mm.
# the minimum overprinting area on copper is 0.6mm.
# the minimum distance between pelable area and pcb edge is 0.5mm.
- it is suggested to put no any peelable material over NPTH or over not-Cu-plated slots or cut off
- it is suggested to reduce the number of peelable not-connected areas so that it will be easier to remove the peelable material after soldering.

Important note: if peelable material is required on both sides of the pcb, it is important to clearly indicate this using 2 different peelable layers, also naming them properly. A clear build-up or layer sequence description in the mechanical layer will be helpful to identify the correct side of the peelable areas

When no any tolerances are specified, the pcb will be produced according to standard tolerance specifications and any way only with PcbOnDemand service different strictly tolerance can be achieved.

Pc Boards CSQPc Boards IPCPc Boards ULPc Boards SofortPc Boards Pay Pal