[geda-user] Silkscreened component values, mailing list, and gEDA development

[mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/]

First, is it possible to design a footprint in such a way that the
component value will appear in the silkscreen, in addition to or instead
of the refdes value? I'm hoping for something more automated than just
manually adding notes to the silkscreen layer.

Second, is there a way to search the archive of this mailing list going
back more than a week into the past? The search function on the archive
page seems to be limited to that, which makes it hard to find previous
answers to questions that have likely been asked before.

Finally, are there any plans for the diode schematic symbols and
footprints to ever agree with each other about which pin is the cathode?
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years. If I
will be required to triple check every symbol and footprint and define my
own a large fraction of the time because there's a significant chance of
the default ones being as catastrophically broken as diodes are, then that
may be a dealbreaking issue and is at least something I'd like to know
about before I invest any more time in gEDA.

[Stephen R. Besch]

Just turn on visibility of the component's value attribute. You can do
this in the footprint itself or in PCB after placement. Then have a look
at the gerber output to be sure it is there

Stephen R. Besch

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
First, is it possible to design a footprint in such a way that the
component value will appear in the silkscreen, in addition to or instead
of the refdes value? I'm hoping for something more automated than just
manually adding notes to the silkscreen layer.
Second, is there a way to search the archive of this mailing list going
back more than a week into the past? The search function on the archive
page seems to be limited to that, which makes it hard to find previous
answers to questions that have likely been asked before.
Finally, are there any plans for the diode schematic symbols and
footprints to ever agree with each other about which pin is the cathode?
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years. If I
will be required to triple check every symbol and footprint and define my
own a large fraction of the time because there's a significant chance of
the default ones being as catastrophically broken as diodes are, then that
may be a dealbreaking issue and is at least something I'd like to know
about before I invest any more time in gEDA.

[mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/]

Just turn on visibility of the component's value attribute. You can do this in
the footprint itself or in PCB after placement. Then have a look at the gerber
output to be sure it is there

How can I do this? I found an "Edit Attributes of... Element" command on
the Edit menu in PCB, but it shows no attributes; the ones defined in the
schematic don't seem to survive translation through gsch2pcb. I can add
attributes manually with that command in PCB, but there is no way apparent
to set them visible; it's just a list of text strings. (They were already
set visible in the schematic, if that helps at all.) And the file format
for footprints doesn't seem to include any way of representing attributes,
so I don't know how I can add them to the footprint.

[Evan Foss]

Yes I have thought that a feature like that would be a good idea. It
should be another column next too the visible checkbox.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/

Just turn on visibility of the component's value attribute. You can do this in
the footprint itself or in PCB after placement. Then have a look at the gerber
output to be sure it is there

How can I do this? I found an "Edit Attributes of... Element" command on
the Edit menu in PCB, but it shows no attributes; the ones defined in the
schematic don't seem to survive translation through gsch2pcb. I can add
attributes manually with that command in PCB, but there is no way apparent
to set them visible; it's just a list of text strings. (They were already
set visible in the schematic, if that helps at all.) And the file format
for footprints doesn't seem to include any way of representing attributes,
so I don't know how I can add them to the footprint.
--
Matthew Skala
http://ansuz.sooke.bc.ca/

[Kai-Martin Knaak]

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
First, is it possible to design a footprint in such a way that the
component value will appear in the silkscreen, in addition to or
instead of the refdes value?

Instead of: yes.
You can switch between any of the three strings "description",
"refdes", and "value" with the menu item:
View --> Displayed_element_name

There is a command for this, too:
Display(foobar)
where foobar is any of "Description", "NameOnPCB", "Value" (without
the quotes) See the pcb manual for details:
http://pcb.geda-project.org/pcb-cvs/pcb.html#Display-Action

In addition: No. Only one of the three strings which are attached
to a footprint can be rendered on silk at a time. This is not as
bad as it sounds. At least in my layouts there is usually hardly
enough space for one string per component, let alone two.

I habitually print two versions of the layout. One with refdeses,
the other with values. See the attached script for a way to do
this automatically with scripted actions. Note, that the script
requires a patch for pcb. Else, the binary will treat the Display()
command in the action script as an error and exits immediately.
(see attachment) Unfortunately, the patch was not accepted by the
devs.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
Second, is there a way to search the archive of this mailing list
going back more than a week into the past?

DJ's setup seems to limit searches to the current week. However,
this mailing list is also archived by gmane.org:
http://dir.gmane.org/gmane.comp.cad.geda.user

The search utility of gmane is quite decent:
http://search.gmane.org/
BTW, the main mission of gmane is to provide a gateway to and from nntp.
his allows the use of usenet readers for the mailing list. Usenet
readers are designed for discussions that involve many authors rather
than just sender and recipient like most emails.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
Finally, are there any plans for the diode schematic symbols and
footprints to ever agree with each other about which pin is the cathode?

Unfortunately, the default library of symbols and footprints went into
some kind of deep freeze about ten years ago. There seems to have been
major fights over the way the library should be designed. As a result,
the default symbol lib is minimal to the point of hardly being useful
for actual day to day work. When I did my first steps with geda in
autumn 2005 there were still repercussions to be felt on the list.
And there were hints to better not touch this topic. People who
complained about the lib were encouraged to roll their own.

In my humble opinion, geda popularity could improve, if there were a
default library of symbols and footprints that are useful for the most
likely work-flow. In particular, symbols should contain footprint
attributes. And of course footprints and symbols should be consistently
designed and proven to work. I started an effort to design such a
library of symbols and footprints:
http://www.gedasymbols.org/user/kai_martin_knaak/essential/essential.html
Unfortunately, the idea did not seem to resonate with the devs.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
there's a significant chance of the default ones being as
catastrophically broken as diodes are, then that may be a
dealbreaking issue and is at least something I'd like to know about
before I invest any more time in gEDA.

I do not use the default libs at all. Over the years I built a pair of
self-consistent libraries of symbols and footprints. See my section at
gedasymbols.org for a preview:
http://www.gedasymbols.org/user/kai_martin_knaak/
However, what you see there is slightly broken in the sense that some
links do not work. This happened because the underlying software CVS
is unable to deal gracefully with rename and/or move of files. However,
my lib grew so much that I felt the need to reorganize the items into
folders with manageable size. I unsuccessfully tried to convince the
CVS repo at gedasymbols.org to accept the new folder structure.

Anyway, if you are interested in a maintained version of my geda
libraries and scripts, you can clone it with git from my repository
at uni-hannover.de:
git clone http://bibo.iqo.uni-hannover.de/git/gedasymbols.git

Hope that helps,

---<)kaiamrtin(>---

[DJ Delorie]

Post by Kai-Martin Knaak
Unfortunately, the default library of symbols and footprints went into
some kind of deep freeze about ten years ago. There seems to have been
major fights over the way the library should be designed. As a result,
the default symbol lib is minimal to the point of hardly being useful
for actual day to day work. When I did my first steps with geda in
autumn 2005 there were still repercussions to be felt on the list.
And there were hints to better not touch this topic. People who
complained about the lib were encouraged to roll their own.
In my humble opinion, geda popularity could improve, if there were a
default library of symbols and footprints that are useful for the most
likely work-flow.

When last we talked about this, we agreed that you would be in charge
of fixing this problem...

[mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/]

Post by Kai-Martin Knaak
You can switch between any of the three strings "description",
designed and proven to work. I started an effort to design such a

Thanks for the links and tips.

[Peter Clifton]

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
Finally, are there any plans for the diode schematic symbols and
footprints to ever agree with each other about which pin is the cathode?

I think diode-3.sym agrees with the ACY series diodes in PCB (or at
least, has reversed pin 1 & 2 from diode-1.sym.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years.

Its not like we can arbitrarily change any of the existing symbols..
doing so would break otherwise working designs.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
If I
will be required to triple check every symbol and footprint and define my
own a large fraction of the time because there's a significant chance of
the default ones being as catastrophically broken as diodes are, then that
may be a dealbreaking issue and is at least something I'd like to know
about before I invest any more time in gEDA.

Can I strongly suggest that whatever tool you end up using, you DO spend
time checking footprint / schematic pin-outs match, hidden power pins
(if any) connect to the nets you expect, and that physical footprints
actually match the components you bought.

Doing all the above is a routine part of designing PCBs that will save
you no end of cost and time where inconsistencies arise. I know
designers who basically throw out huge component libraries from big
commercial EDA vendors, because they are not reliable enough to trust
out of the box.

If you haven't found it yet, http://www.gedasymbols.org/ is a useful
place to find and share symbols for gEDA.

[mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/]

Post by Peter Clifton

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years.

Its not like we can arbitrarily change any of the existing symbols..
doing so would break otherwise working designs.

Is that really true? At least on the PCB side, changes to footprint files
don't seem to take effect on a board unless the user goes through a
laborious process to manually replace them one by one.

[gedau-1XeMD6fE9sqV9CSZFf/]

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/

Post by Peter Clifton

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years.

Its not like we can arbitrarily change any of the existing symbols..
doing so would break otherwise working designs.

Is that really true? At least on the PCB side, changes to footprint files
don't seem to take effect on a board unless the user goes through a
laborious process to manually replace them one by one.

It is different in gschem.

In short: gschem default is external ref and you can embed the symbol. In
pcb you always embed, there's no other option afaik.

Regards,

Tibor

[mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/]

Post by gedau-1XeMD6fE9sqV9CSZFf/

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
Is that really true? At least on the PCB side, changes to footprint files
don't seem to take effect on a board unless the user goes through a
laborious process to manually replace them one by one.

It is different in gschem.

Well then, the footprints could change to match the symbols instead of the
other way around. But it sounds like my question has been answered and
there's not much purpose served by continuing to discuss this point at
this time.

[Peter Clifton]

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/

Post by Peter Clifton

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years.

Its not like we can arbitrarily change any of the existing symbols..
doing so would break otherwise working designs.

Is that really true? At least on the PCB side, changes to footprint files
don't seem to take effect on a board unless the user goes through a
laborious process to manually replace them one by one.

True, PCB does hard-copy the symbol into the .pcb file, but if we
changed the library at some arbitrary point, it would mean any newly
transferred symbols would then not match existing ones.

It might not affect people on legacy designs, but you will always catch
people with things still in progress.

The only way we can acceptably change this kind of thing is:

1) Rip out all libraries (very obvious to users) and start again
2) Add new, distinct symbols and footprints to the existing libraries


We were at one point planning to do 1), replacing gschem's symbol
library with a minimal, schematic biased library of primitive devices
(eg. "DIODE", not 1N4002 etc..). We had also talked of mapping between
generic symbols (DIODE with A&C PINS, transistors with B,C,E), into
pin-numbers for actual components, but this never happened. We just
don't have the resources to produce a huge vetted library like the big
commercial tool vendors do.

[John Doty]

Post by Peter Clifton
We just
don't have the resources to produce a huge vetted library like the big
commercial tool vendors do.

And, having used the $30k/seat/year stuff, I have to say that it wasn’t any better. Lacking firm standards for pin numbering, the problem cannot be solved in the general case.

John Doty Noqsi Aerospace, Ltd.
http://www.noqsi.com/
jpd-***@public.gmane.org

[John Doty]

Post by Peter Clifton
I think diode-3.sym agrees with the ACY series diodes in PCB (or at
least, has reversed pin 1 & 2 from diode-1.sym.

Screaming Circuits recently stopped checking diode pin numbers against schematics, resulting in a bunch of boards with reversed diodes. They told my customer that "the convention" is that cathode is pin 1. Perhaps there is an emerging defacto convention, although I’m not aware of any standard.

Most of the symbols in the library predate the shotgun marriage between the gEDA and pcb projects, so of course there are inconsistencies. The library symbols were created at different times by different people for different design flows. Their creators generally did not understand flows they were not using. Nobody knows how to make a symbol that supports every flow.

For SPICE, the anode comes first, so it should have pinseq=1. diode-1.sym and diode-2.sym are correct, but diode-3.sym and schottky-1.sym are wrong. Many symbol creators don’t seem to understand pinseq.

John Doty Noqsi Aerospace, Ltd.
http://www.noqsi.com/
jpd-***@public.gmane.org

[Britton Kerin]

Post by John Doty

Post by Peter Clifton
I think diode-3.sym agrees with the ACY series diodes in PCB (or at
least, has reversed pin 1 & 2 from diode-1.sym.

Screaming Circuits recently stopped checking diode pin numbers against schematics, resulting in a bunch of boards with reversed diodes. They told my customer that "the convention" is that cathode is pin 1. Perhaps there is an emerging defacto convention, although I’m not aware of any standard.
Most of the symbols in the library predate the shotgun marriage between the

Not shotgun marriage. Normal healthy consensual sex.

Post by John Doty
gEDA and pcb projects, so of course there are inconsistencies. The library
symbols were created at different times by different people for different
design flows. Their creators generally did not understand flows they were
not using. Nobody knows how to make a symbol that supports every flow.

This is always the excuse for the bad state of the symbol libraries. But 98%
of the time there is no reason to change the footprint/mask/stencil etc.
for a given part, and the most common flow by far is gschem->pcb. Nor is
there any reason having that flow work gracefully should prevent other custom
stuff from working.

Of course we can't produce a full coverage symbol library. As you point
out previously that approach is fundamentally flawed anyway: its pretty much
guaranteed to result in a bunch of untested buggy heavy symbols.

What we could in theory achieve is a set of tested prototypes from which people
could pick and choose, and some systematic way to tweak existing symbols to
quickly produce what is needed. The trouble is everyone who cares already
has their own library and system for producing new symbols from prototypes.
Kai's way doesn't sound good for me and I'm pretty sure he would hate mine,
but there's probably no real reason for this other than their independent
invention. Sad.

Britton

[Vladimir Zhbanov]

Post by John Doty

Post by Peter Clifton
I think diode-3.sym agrees with the ACY series diodes in PCB (or at
least, has reversed pin 1 & 2 from diode-1.sym.

Screaming Circuits recently stopped checking diode pin numbers against
schematics, resulting in a bunch of boards with reversed diodes. They
told my customer that "the convention" is that cathode is pin 1.
Perhaps there is an emerging defacto convention, although I’m not
aware of any standard.

There is at least an IPC standard.
You can find at http://landpatterns.ipc.org/IPC-7351BNamingConvention.pdf.
See p.5 for numbering conventions. They seem to follow IEC standards,
but I'm in doubt since I found no IEC convention on pin numbering yet.

I've also found a link to the full version of the standard. See it at
http://pcbget.ru/Files/Standarts/IPC_7351.pdf. Pin numbering examples
start at page 66.

We could follow that standard in regard to gschem->pcb workflow.

Post by John Doty
For SPICE, the anode comes first, so it should have pinseq=1.
diode-1.sym and diode-2.sym are correct, but diode-3.sym and
schottky-1.sym are wrong. Many symbol creators don’t seem to
understand pinseq.

For SPICE, I'm thinking of using a unique attribute, say "pinnode". So we
could part the two workflows - simulation in SPICE and making pcb's.
I believe that in general every particular workflow should lean on its
own attributes in gEDA/gaf.

Vladimir

[Stuart Brorson]

Hi --

Post by Vladimir Zhbanov

Many symbol creators don?t seem to
understand pinseq.

For SPICE, I'm thinking of using a unique attribute, say "pinnode". So we
could part the two workflows - simulation in SPICE and making pcb's.
I believe that in general every particular workflow should lean on its
own attributes in gEDA/gaf.

Overloading pinseq for use with spice-sdb seems to have caused a lot
more grief than I could have imagined at the time. I think the idea
of separating the workflows makes sense. Moreover, eliminating the
overload would be a good thing. I would do it be modifying spice-sdb
to use a different atribute, for example pinnode, as you say. Or
spicepin, or something like that.

The only question is, how many legacy schematics would you break?
IMO, I don't think that many folks keep gEDA simulations going for
years and years. And those who do are very clueful and will know how
to fix their spice schematics using grep and other tools. Therefore,
breaking legacy work is probably not a show stopper.

I say, go for it.

Stuart
Original spice-sdb developer.

[John Doty]

Post by Stuart Brorson
Hi --

Post by Vladimir Zhbanov

Many symbol creators don?t seem to
understand pinseq.

For SPICE, I'm thinking of using a unique attribute, say "pinnode". So we
could part the two workflows - simulation in SPICE and making pcb's.
I believe that in general every particular workflow should lean on its
own attributes in gEDA/gaf.

Overloading pinseq for use with spice-sdb seems to have caused a lot
more grief than I could have imagined at the time. I think the idea
of separating the workflows makes sense. Moreover, eliminating the
overload would be a good thing. I would do it be modifying spice-sdb
to use a different atribute, for example pinnode, as you say. Or
spicepin, or something like that.

See https://github.com/noqsi/gnet-spice-noqsi. Its spice-prototype attribute is very flexible. It controls refdes munging, connections, parameters, etc. Connections can be ordered by pinseq or in arbitrary order by pinnumber (much handier for slotted components). If you turn off gnetlist’s hierarchy expansion, spice-noqsi can turn hierarchical blocks developed for layout into SPICE subcircuits, and interpret the corresponding symbols correctly. Here’s an example of a “test fixture” for a subcircuit. The symbol and the underlying source schematic (which, unfortunately, I cannot publish) don’t change *at all* when I use them in a printed circuit netlist flow.

[Dan McMahill]

Post by Peter Clifton

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
Finally, are there any plans for the diode schematic symbols and
footprints to ever agree with each other about which pin is the cathode?

I think diode-3.sym agrees with the ACY series diodes in PCB (or at
least, has reversed pin 1 & 2 from diode-1.sym.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
I have found bug reports about this dating at least as far back as May
2005, but nothing seems to have been done about it in nine years.

Its not like we can arbitrarily change any of the existing symbols..
doing so would break otherwise working designs.

Post by mskala-iYp5QZLjffFsCj9YYT8S7fd9D2ou9A/
If I
will be required to triple check every symbol and footprint and define my
own a large fraction of the time because there's a significant chance of
the default ones being as catastrophically broken as diodes are, then that
may be a dealbreaking issue and is at least something I'd like to know
about before I invest any more time in gEDA.

Can I strongly suggest that whatever tool you end up using, you DO spend
time checking footprint / schematic pin-outs match, hidden power pins
(if any) connect to the nets you expect, and that physical footprints
actually match the components you bought.
Doing all the above is a routine part of designing PCBs that will save
you no end of cost and time where inconsistencies arise. I know
designers who basically throw out huge component libraries from big
commercial EDA vendors, because they are not reliable enough to trust
out of the box.
If you haven't found it yet, http://www.gedasymbols.org/ is a useful
place to find and share symbols for gEDA.

The issue of a reliable symbol/footprint library is one that is there on
all systems. I've been burned by using the bundled library on a very
high dollar system before. The problem with a diode is this. Diodes
come in many many different packages. Unless every one of those
packages agrees on which is pin 1 (anode or cathode) (and they neve
will) then using a generic symbol for the diode will eventually cause a
problem. This is why I tend towards the approach of a symbol per
complete part number (including the package codes) that is attached
correctly to the footprint with the pin out correct. I used a fairly
simple build system to help generate all of those symbols from a
template symbol and a text database. It is some effort but the result
is symbols I can trust. Of course I haven't had time in several years
to do any board designs so my library reflects that. If you're
interested though it should be up on gedasymbols.org.

http://www.gedasymbols.org/user/dan_mcmahill/

Among the many problems is that you won't even find universal agreement
across vendors on how package pins are numbered. For example:

# ___x_
# / \
# TO18: |3 1| <-- bottom view (supposed to be a circle)
# \ 2 /
# ---
# NOTE: Philips and ST number their TO-18's differently.
# I will use the JEDEC numbering which is what Philips uses.

SOT-23's are notorious for this as well.

Others have other approaches but for me having an ascii database that
defines the mapping between symbol pins and footprint pins for each
complete component has worked reasonably well.

-Dan (now returning to the rock I've been hiding under)

[gedau-1XeMD6fE9sqV9CSZFf/]

Post by Dan McMahill
SOT-23's are notorious for this as well.
Others have other approaches but for me having an ascii database that defines
the mapping between symbol pins and footprint pins for each complete component
has worked reasonably well.

I have a similar setup and it works very well. Mine has two stages:

1. pinmap attribute: name=number pairs, e.g. "pinmap=G=1;S=2;D=3" for a
mosfet where G, S, and D are pin names on the gschem symbol and 1, 2 and 3
are pin numbers in pcb

2. a set of small text files named as "device_footprint", e.g.
"2n7002_sot23" and a "devmap=filename" attribute on the schematics. The
files contain generic attribute rewrite directives, usually setting up
pinmap and footprint attributes.

I have a wrapper around gsch2pcb that first executes the devmap attributes
using a predefined directory as database, then it applies the pinmap
attributes to renumber pins.

Pros:
- very easy to maintain the library of mappings - no complicated database
software, gui, custom version control, but my favorite text editor and my
favorite VCS
- easy to follow and manually tweak the process
- because of the generic attribute rewrite, it can potentially do more
than just map pinouts
- very easy and fast to use: instead of footprint, I just assign a devmap
attribute and I know I won't have to worry about the footprint and pinout
- can use generic light symbols from any source as long as pins are
named; can use the same symbol for different models/packages within the
same schematics

Cons:
- the major drawback is that the schematics does not show actual pin
numbers (may be a problem while debugging the circuit)
- the implementation is hackish: gschlas, a set of scripts
- I have to remember to use the wrapper version of gsch2pcb


Regards,

Tibor