Mail Archives: geda-help/2019/10/22/18:15:08
John L. Males (jlmales AT gmail DOT com) [via geda-help AT delorie DOT com] wrote:
> The Pin statement in the 3x6 hole part I created as one
> example was:
>
> Pin(300 350 125 90 "101" 0x01)
>
> Your great example to make it a pure hole with no connection
> attribute was:
>
> Pin[0 0 3.6mm 0.4mm 3.4mm 3.2mm "" "1" "hole"]
>
> If there a difference in context or meaning of the Pin
> statement when using round brackets vs square brackets?
If I understand your question correctly then the answer is no;
they both create the same thing on the board.
> There is a difference in the number of items I used from the
> connector part I used as basis of my pin statement. Is this
> related to the type of brackets used as asked just above?
Yes. Here's the documentation:
http://pcb.geda-project.org/pcb-cvs/pcb.html#Pin-syntax
> Am I correct to assume the first two zeros you used are still
> for the pin location?
Yes.
> If one does not use the "mm" units suffix in your example will
> that mean the default units is mils?
I think so, but I'm not sure.
> Can one explicitly state mils a a unit of measure?
Yes.
> One aspect I learned was the use of 0x101 in the format of the
> Pin statement created a square hole and graphic inside that
> collectively indicate pin 1 of the connector. Is this the same
> parameter in the round brackets syntax I deduced from a
> connector part that can indicate hole?
Yes. The square bracket syntax allows using symbolic flags, more
human readable.
The "square" symbolic flag (combine flags using a comma) doesn't make
much difference for a Pin with the "hole" flag.
The "square" flag doesn't create a square hole, but results in a
square copper pad, as often seen for pin 1.
> The second and third value in the round bracket Pin syntax I
> deduced from the connector part were outside and inside
> diameter.
Yes, Thickness and Drill.
> The first 4 values of the round bracket Pin syntax I used are
> in mils as I discovered.
Yes.
> I am assuming the 5th value in the round bracket values I used
> is some sort of comment or reference point that I do not see in
> the PCB nor gerbers I created as test.
Yes. It's the name of the pin. Not relevant for your ventilation
holes, but can be helpful for anything that connects somewhere.
Names can be displayed in the GUI, and are sometimes used in
messages.
> The current indications I have states the boards have a capacitance
> between 27pF to 39pF.
Doesn't that depend completely on copper area and dielectric constant
(meaning thickness, and uniformity)?
I assumed that you have a target capacitance which you need to achieve.
Another option could be to create a 4-layer board with a quite thin
core and no copper on the two outermost layers, which probably allows
another capacitance range and perhaps significantly tighter tolerance.
> I believe the wide tolerance is due to using FR4 boards.
I have no idea; I don't know where the number 27-39pF comes from. :)
> I think it was Chad that mentioned Polyimide board that my sense
> was would have smaller capacitance tolerances including from
> temperature delta point of view.
PI is one choice, but will probably be very thin at most fabs - this is
the core used for all flex PCBs - the copper-coloured bendy PCBs that
are inside many things with moving parts.
> Thickness is also a factor because the gap this sensor board
> sits between is about 0.125". So a board that is also
> dimensionally stable is important as well. The fixtures the
> board is attached to are of a warp less design.
A board will never reliably fit snug into that gap, so make sure that
there is a separate mount for the PCB. Check if mounting force warps
the board enough to affect capacitance in a relevant way.
> The board does not move, but maybe the metal it is mounted to
> might pinch the solder mask that would cause unwanted low
> voltage short that wold render the sensor board useless as well
> as the application. I had been considering before your comment
> about the solder mask if running a trace or making a small gap
> about a via at edge of the copper planes to transition the
> lower connection to upper side of board that is not in contact
> with metal fixture to then run the trace top side to the solder
> pad.
Yes. Avoid copper on the board underneath the metal mount.
> Is it possible to make a copper area a part?
From http://pcb.geda-project.org/pcb-cvs/pcb.html#Element-syntax
"Elements may contain pins, pads, element lines, element arcs,
attributes, and (for older elements) an optional mark."
So no, no polygons. pcb-rnd allows that, but only using its own file
format.
> Why is it important to provide at least a 0.5mm space of copper
> from side of the board?
The fab will route the outer edge of the PCB, again with some tolerance.
The 0.5mm space ensures that no copper will extend to the edge of the
board, which could result in a short circuit if that edge touches some
surrounding metal.
Also, soldermask doesn't always extend to the very edge. Leaving space
without copper also ensures that all copper is actually masked.
And some fabs do not route the outer edge completely, but leave a few
bridges or tabs perforated with small drilled holes along the outer
edge of your design, so that those tabs can be broken off easily in
the very last fabrication step. The holes extend "into" your board,
and the break-off process can tear the soldermask and crack the core
imperfectly or unevenly. That shouldn't cause exposed copper.
> If not could one edit the text file of the board with
> the copper sides on it manually to effect the at least 0.5mm
> clearance of copper from the edge of the board.
Mh, yes sure, but it's not so convenient.
> Do this via the GUI is challenge as one would have to zoom the board
> so much it may make trying to effect the clearance from the edge
> challenging or not practical from a GUI point of view.
The GUI has a grid which helps a lot for such operations.
> I have skipped questions I have of the "Element" statement and
> "ElementLine" for now until I have the "Pin" statement
> questions I asked above sorted out that I understand for my
> needs.
Maybe your questions are already answered in the documentation. :)
//Peter
- Raw text -