The paste layer artwork is used to make a paste screen (nowadays
usually stainless steel, although sometimes brass) through which
a stencil printer can squeegee solder paste.

The stencil printing process is like a silkscreen on steroids.
The stencil is aligned (usually optically) to the incoming PCB, then
the pressed down against the PCB. The squeegee (usually a spring
steel blade) passes over the screen, forcing the solder paste (which
is composed of size-controlled balls of solder alloy in a flux
suspension) down into the holes in the screen.

The thickness of the screen, plus the aperture size, determines the
volume of paste deposited (too little = bad joints with inadequate
fillets of solder; too much = solder bridges (shorts)). The geometry
of the aperture (peripheral circumference:area) has a large effect
on the ability of the past to snap away from the screen and stick to
the PCB when the screen is lifted off after the squeegee pass.

The paste layer is different from the solder mask layer for two
main reasons:

1/ Whereas the solder mask has openings for all pads, solder paste
needs only to be deposited for surface mount components that are going
through a reflow process. (Some companies use paste deposition for
through-hole component leads too, but it's far from universal
practise).

2/ There is often a need to control the paste screen aperture size
based on the component type to ensure correct volume and aspect
ratio.

The twiddling of the apertures is usually done by the assembly house
(or their screen manufacturing contractor), so the PCB designer
doesn't usuallly need to be too concerned with paste mask expansions,
etc.

I would really recommend personally visiting both a PCB fabricator and
a contract assembly house, so that you can get a real feel for the
process flows.

John Haddy

-----Original Message-----
From: Waheed Bajwa [mailto:[EMAIL PROTECTED]]
Sent: Friday, 17 May 2002 7:24 PM
To: Protel EDA Forum
Subject: Re: [PEDA] Some more info


Well Ian thats a lot of useful information and of great help to me... and
thanx for the link too...

Just a few clarifications...

So the overlay layer and the silkscreen layer is the same thing...
Looks like the mechanical layers are not invovled in the manufacturing of
PCB and just for reference only? no conduction?

I get what is Solder Mask layer but what I don't get is why do we need paste
layer after this? I blv both are almost the same thing... There would be
holes in the solder mask layer and there we can apply the paste even if its
the case of surface mounted components... Please explain...

Best Regards,
Waheed Bajwa

==================================
Design Engineer
Communications Enabling Technologies
Software Technology Park,
5-A Constitution Avenue,
Islamabad - 44000
Pakistan
Ph. No: +92-51-2826160 Ext. 254
http://www.enabtech.com
==================================

----- Original Message -----
From: "Ian Wilson" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Friday, May 17, 2002 12:42 PM
Subject: Re: [PEDA] Some more info


> On 12:16 PM 17/05/2002 +0500, Waheed Bajwa said:
> >Ok here are some more information requiring issues...
> >
> >What is:
> >
> >Top/Bottom Paste layer
>
> One method of soldering components to a PCB is by a reflow technique where
> a small amount of solder paste (solder balls in a evaporating carrier) is
> put on the boards.  Where do you put the solder - where there are holes in
> the mask.  The mask or paste screen is a thin sheet of metal (stainless or
> brass usually) with holes where the paste should be applied.  For details
> on how try to get into a assembly plant and get them to show you.  In some
> cases the paste is no longer applied with a screen but the terminology
> remains.  The paste layers are
> negative layers.  That means that where you see something on your screen
> (on this layer) there will be a gap in the mask and so solder paste will
> apply there.  Solder paste is usually only applied to surface mount
> pads.  In Protel there are "automatic" paste layer gaps on the matching
> layer for surface mount pads.  So a Top layer pad will automatically have
a
> matching hole in the top paste mask (similarly for bottom layer/bottom
> paste).  You can, of course, control the the expansion of the paste gap
> (either larger or smaller) compared to its matching top/bottom pad.  You
> can also put your own tracks an fills on the paste layer to apply extra
> paste in the regions of your tracks/pads - but this is usually not
necessary.
>
> Protel knows that tracks on the paste layers do not carry signals and they
> therefore do cause any short circuits for the DRC.
>
> >Top/Bottom Solder layer
>
> Grab a finished PCB - or open a computer.  See the green covering (usually
> it is green) - that is the solder mask (I assume that is what you are
> talking about).  Almost all the comments about paste mask apply to the
> solder mask (its negative nature, non-electrical etc).  it is designed to
> stop shorts between copper tracks and to reduce the corrosion of the
copper.
>
> >Drill Guide layer
> >Drill Drawing layer
>
> In nigh on 20 years of PCB work I have never ever used the drill guide -
it
> basically shows you where the pads are but it is rarely used.  the drill
> drawing layer is also less used these days but much more than the Drill
> Guide layer.  The thing about these layers is that are for information
only
> - nothing on them is conductive or appears on the PCB.  They were used to
> communicate the locations of drill holes and their sizes.  This is
commonly
> done these days with a separate drill file which is loaded into a CNC
drill.
>
> >Silkscreen
>
> Grab that PCB again - see the white (usually) text.  That is the
silkscreen
> layer (one for top and one for bottom). Put text on there and it will be
> visible on the board. It is not conductive.  Be careful to try hard not to
> get silkscreen text and other graphics onto pads and vias - try to keep
the
> silkscreen on the areas of solder mask.
>
> >Part Numbers layer
> >Template_Dimensions layer
>
> These two are not actual Protel layers - but you are able to set up a
> couple of mechanical layers to act as these layer is you want.  the
> mechanical layers are non-electrical and can be used as you wish for
things
> like dimensions, manufacturing notes etc.  Typically Mech Layer 1 is used
> to show the PCB outline and the other mech layers used for other
> information purposes.  The KeepOut Layer is sometimes used to show the
> board outline but I really do not like this - the keep out should really
be
> used to define where tracks and components can go - usually not to the
very
> edge of the board.  The keepout will often be a mm or more inside the
board
> outline - the keepout is used to define where stuff parts and copper can
> go.  It is checked by the DRC and you are warned of encroachments.  This
is
> not the case with mechanical layers.
>
> As a basic readily available primer of PCBs and their construction have a
> look at:
> http://www4.tomshardware.com/howto/01q3/010810/
>
> Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to