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