Re: [PROTEL EDA USERS]: Special Solder Paste

["Geoff Harland" <gharland@ingenico.com.au>]

> The method I use is to mask the pad completly (ie set
> the soldermask expansion to at least -(1/2 the max
> dimension). Then place a fill on the soldermask layer.
>
> Simon
>
> > > I need to offset and make the solder paste pads
> > smaller on chip components.
> > >
> > > Can anyone please make suggestions?

The right idea, but the originator of this thread requested how to get
offset pads on the Solder *Paste* layer. As such, the (copper layer) pad
should be masked on the Solder Paste layer, which is achieved by setting the
Solder Paste expansion value to a sufficiently negative value. However,
choosing a (negative) value whose (absolute) value is at least equal to the
*smaller* of the (copper layer) pad's dimensions will suffice; it is not
necessary (but won't hurt) to choose an (absolute) value that is equal to or
larger than the *larger* of the (copper layer) pad's dimensions (in the
event that these dimensions differ, of course).

Similarly, the fill should be placed on the Solder Paste layer. However, a
fill can be used for this purpose only if the shape of the image required on
this layer is rectangular (or square) in shape. Otherwise, a pad should be
used for this purpose (and assigned appropriate dimensions and shape, and
placed in the appropriate location).

And as I have mentioned in assorted past postings, I strongly advocate that
*every* pad within a footprint be assigned an *unique* (*and* non-null)
designator (/number), including any pads placed on the Solder Paste (and/or
Solder Mask) layer(s). (Something of a hobby horse of mine, but a practise
that can save you some grief.)

To expand upon the original thread slightly, (copper layer) pads which are
used as fiducials should normally be masked on the Solder Paste layer. There
are other (copper layer) pads which should similarly be masked, such as the
gold-plated "finger" contacts in (built-in/intrinsic) edge connectors (where
you would typically use pads with an obround/oval shape). Because of the
usage of such pads, I have previously suggested to Protel that the
"Advanced" Tab in the "Pad" dialog box should include a "Tenting" check box
for not just the Solder Mask (expansion setting), but *also* the Paste Mask
(expansion setting). So until (and if) Protel implement this, users wanting
to mask a (copper layer) pad on the Paste Mask layer should set its (Solder
Paste) expansion value to a sufficiently negative value, as described
earlier in this post.

Regards,
Geoff Harland.
-----------------------------
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.