> well, thats a pretty dumb question, isn't it?  hahaha.
> but i'm serious.  i'm trying to reproduce a board which
> has smt top and bottom, and it appears that some of the
> smt pads overlap from top to bottom.
>
> so how do smt pads work?  on a thru-hole, they obviously
> go thru the entire board.  how far does a pad go thru as
> an smt?  obviously it has to at least burrow thru to any
> layer it runs on, but do top and bottom overlapping smt
> pads necessarily net together?  i'm confused.
>
> let me state that i realize many complex things are
> possible (blind and buried vias come to my mind), but
> somehow i don't think this is the case with this board.
> but i'm not sure.
>
> thanks, miker

In Protel, pads on the MultiLayer layer occupy all copper layers on the PCB.
Assuming the (pad's) hole diameter is not zero, there are also (anti)pads on
the internal power plane layers. (Those (anti)pads are always circular in
shape, because the hole is circular in shape.)

Pads on all other layers occupy that layer only (with the qualification that
pads on the outside copper layers are "imaged" on the Solder Mask layer and
Paste Mask layer on the same side of the PCB as the pad; pads on the
MultiLayer layer are similarly "imaged" on both Solder Mask layers (but
neither Paste Mask layer)).

Pads have a "padstack" feature, but this is only relevant for pads on the
MultiLayer layer; this feature permits the shape and dimensions of the pad
to be customised for each of the (outside) top signal layer, the (outside)
bottom signal layer, and the remaining (internal) signal layers. IMO, that
feature should be disabled for pads on any other layer, as only one of those
three sets of properties is relevant for such pads (with the other two sets
of properties being of no practical significance).

(Advance information is that the "padstacks" feature is going to be enhanced
in Phoenix; I am hoping this won't be buggy in nature.)

All pads can have an associated hole, but while it is not compulsory, it is
still extremely advisable to set the hole diameter to zero for all pads
which are not on one of the external copper layers or MultiLayer layer, and
I personally would be reluctant to have holes in pads even on either of the
external signal layers.

All pads also have a "Plated" property; IME, it is advisable to always set
this True unless the pad is on the MultiLayer layer and you *don't* want
this through plated. (Again, this property should always be disabled if the
associated pad has a zero diameter hole.)

It's almost certainly too late in the piece for incorporation in Phoenix,
but my opinion (which I have distilled over time) is that all Pad objects
should exist solely on the MultiLayer layer, and be of either a Top Surface
Mount type, or a Bottom Surface Mount type, or a Through Hole type;
regardless of which of these types each pad is, it occupies more than one
layer, to wit one Solder Mask layer and one Paste Mask layer for SM pads,
and two Solder Mask layers for ThroughHole pads (though there would be merit
in also being able to "image" such pads on each of the Paste Mask layers as
well). In lieu of "Pad" objects on other layers, there should be enhanced
"Fill" objects on other layers; these enhanced "Fill" objects would be like
existing Fills in that they would never be "imaged" on any other layers, and
with the enhancement being that a "Fill" could either have a Rectangular,
Obround, or Octagonal shape (rather than just a Rectangular shape as at
present). The (new) dialog box for Fill objects would permit one of these
shapes to be selected, and the user would also have the option of being able
to specify the region occupied by the Fill either by the use of Low and High
X and Y co-ordinates (i.e. like existing Fills), or alternatively by
co-ordinates for the centre, and Width and Height properties (i.e. like
existing Pads). (Both sets of properties would be displayed, but two radio
buttons would also be provided to select which set of properties is *just*
displayed and which set of properties is not just displayed, but also
editable. Alternatively, just one set of properties is displayed at a given
time, and these are editable, but selecting the other radio button would
then change the set of properties displayed.)

It goes without saying that such SM pads should not be displayed unless they
exist on a layer which is currently selected for displaying. (At present,
there is a bug in that blind or buried vias are displayed even when these do
*not* exist on layers which are currently displayed.)

(I have previously stated that I believe that Vias should remain a distinct
type of object from Pads, because otherwise it would not be possible to
create "Pad Master" type printouts or Gerber files. That said, there is
still a case for enhancing the ability to control Vias' properties, so that
(as at least one example) designers can select masking of vias on one side
of the PCB, but not on the other side.)

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.



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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