The differences between various PCB layers

[SphinX]

Hi,

I want to know what is the difference between these layers

TOP ASSY
TOP PASTE
TOP MASK
TOP SILK

What is meanning of ASSY, PASTE AND MASK ?

Thanx

 

[Sukohi_Berkut]

solder paste layer

TOP ASSY
Assy - Assembly layer
This is used for the assembly people who place and solder the components. This is similar to silk-screen print but it may include the pins of the component and large reference designator for easy identification.

TOP PASTE
This gerber is used to create a stencil. the automated placeing machine will place all the surface mount components before taking them to the reflow solder machine.

now to secure the components with their respective land-pattern a adhesive is used.

this paste layer will have only the land pattern opening and using this a stencil will be made on a steel plate.

that stencil will be placed over the bare pcb and a glue will be applied over them.

now when u place a compnent on its place, the glue will allow it to stay put for the soldering place.

TOP MASK

This is solder-mask layer, all solderable pads has a extra clearance than its pad size, to allow the tolerance for the soldering.
in other words in this extra clearance there won't be any solder mask. ie open

TOP SILK

This is the silk-screen layer, this will be on the pcb and it includes the component outline, ref-des
regards

 

[cyberrat]

paste mask pcb

IMO Top paste should be used for solder paste, not glue. Top Glue should be used for that. But if thats how you create a glue screen then I bow to your use of it as I have never actually used glue (nasty sticky stuff!).

The paste stencil has apetures in (holes) equal or smaller than the SMT pads so that solder paste can be applied to them using a solder pasting machine (be it automatic or manual) before it is sent through the placement machines.

It is common for the pads/apetures/holes to be reduced by about 10% so that there is less solder paste on the pad, this helps to prevent solder balls etc. The amount of reduction is depentant upon the manufacturing process itself.

As for the top mask layer, this is the solder resist (green stuff) clearance around the pads. if you can assign a different sized pad to this layer you can make the clearance already without having to add it during photoplotting.
A clearance of aprox 8 thou is normal.
It is also a useful layer to add figures etc in the solder resist I.E. a strip of solder resist through the land of a non PTH mounting hole on the bottom copper can often help avoid the hole filling over during wave soldering.
For VIA's you can make the pad size zero on this layer so that they are under the masking (assuming you cannot turn them off) or in fact you can give some of them larger pads to allow them to be filled but other zero so that they are not. (filling via's is another matter altogether).

I would suggest that you have a good look into the uses of your layers, what facilities are available through them and define a standard use for each, then stcik to the same naming conventions etc. That way any macro's or batch processing will work with them all.

Oh, and have a good Christmas..

Roland.

 

[Sukohi_Berkut]

pcb paste layer

hi cyberrat
thx for the corrections and detailed explanation

I never created a glue layer, i use paste layer for stencils
regards
merry xmas and happy new year to all