Re: gEDA-user: Matching footprints with symbols
Colin D Bennett wrote: Bottom line: Avoid hyphens in footprint names except to add a revision number at the end of the base name. Alternate bottom line: Avoid m4 footprint library. ack. In addition: Be aware of potential problems if you share your hyphenated footprints with other users. I ran into this problem back, when I used some of the footprints, John Luciani generously provides on his home page. nag-mode When is this newbie trap going to be defused? /nag-mode ---)kaimartin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Mon, 15 Nov 2010 14:56:09 +0100 Kai-Martin Knaak kn...@iqo.uni-hannover.de wrote: Colin D Bennett wrote: Bottom line: Avoid hyphens in footprint names except to add a revision number at the end of the base name. Alternate bottom line: Avoid m4 footprint library. ack. In addition: Be aware of potential problems if you share your hyphenated footprints with other users. I ran into this problem back, when I used some of the footprints, John Luciani generously provides on his home page. But if the footprints in question (with names containing hyphens) are in newlib (PCB element) format, doesn't this mean that the m4 processor bug will be avoided? Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Colin D Bennett wrote: But if the footprints in question (with names containing hyphens) are in newlib (PCB element) format, doesn't this mean that the m4 processor bug will be avoided? Unfortunately, not. By default, gsch2pcb hands all footprints to the m4 processor. There is an option to skip m4 for good, though (--skip-m4). But unless the option is given, hyphens in footprint names result in broken pcb files. The breakage does not show immediately, but usually somewhere down the work flow. ---)kaimartin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Stefan Salewski wrote: On Sat, 2010-04-17 at 01:15 +0200, Armin Faltl wrote: Did anyone try my schematic posted in http://www.seul.org/pipermail/geda-user/2010-April/046716.html I read the list with knode via gmane. Unfortunately, gmane munged your attachments. And I was too lazy to ask for a resend to my private email address. One remark: You used the minus sign - in your footprint names. This seems to be the initiation bug for serious geda users :-P Welcome to the club! Seriously, this bug is long standing since at least eight years. It has been discussed multiple times on the list and even been ranted on. The bug itself has not been addressed, yet. Some (power) users make a point in never using the m4 lib directly -- Most notably John Luciani. They thus can get away with hyphens in their footprint names. There is an option to gsch2pcb to ignore the m4 library no matter what: --skip-m4 This can give trouble in rare cases due to m4 macro expansion. /rare/many/ The insidious side of this bug shows by the many seemingly unrelated ways it breaks the layout further down the road. Bottom line: Avoid hyphens in footprint names except to add a revision number at the end of the base name. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
kai-martin knaak wrote: Bottom line: Avoid hyphens in footprint names except to add a revision number at the end of the base name. For some reason, this posting got stuck in the outbox when more than 6 months ago. Now, it finally got unleashed. Sorry for the inconvenience. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sat, 17 Apr 2010 05:23:05 +0200 kai-martin knaak k...@familieknaak.de wrote: Stefan Salewski wrote: This can give trouble in rare cases due to m4 macro expansion. /rare/many/ The insidious side of this bug shows by the many seemingly unrelated ways it breaks the layout further down the road. Bottom line: Avoid hyphens in footprint names except to add a revision number at the end of the base name. Alternate bottom line: Avoid m4 footprint library. Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sat, 2010-04-17 at 13:25 +0200, Stefan Salewski wrote: On Sat, 2010-04-17 at 13:10 +0200, Stefan Salewski wrote: On Sat, 2010-04-17 at 12:37 +0200, Stefan Salewski wrote: I think I have to rename all of them, including John Luciani's. You have components in your schematic named Rf and Cf without numbers. These seems to have no connection in the netlist. The missing number in refdes seems to be a problem. OK, seems to be all fixed now, see http://www.ssalewski.de/tmp/armin20100417.tar refdes without a digit at the end of the name seems to be indeed a big problem, I am not sure if this is stated at a prominent location in the gEDA/PCB documentation? Specifically, it is the _lower case_ letter at the end which is ignored. It was a (mis)feature designed to support IC1a IC1b as the same part, IC1 in the netlist. I don't think upper case letters at the end of a refdes (without a number) cause a problem. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
I made a first attempt to create a database schema, that's a collection of table definitions on this - It's not a good idea to work on tables representing trees and DAG's at 02:00 in the morning, so this is just sketches and reminders of what I want. Some other list member is working in the same direction. Usually I start with a requirements specification if doing serious dev and this would go for review here or at least some peers. Once I got something presentable, I'll present it ;-) Vladimir Zhbanov wrote: Armin Faltl wrote: Hello Vladimir, the point in not using a text file format for this but a relational database with SQL is not the data storage but the capabilities of the database server. It allows modeling of relations and more important, relational queries. This can look something like: SELECT elem.footprint FROM elem, part WHERE part.name LIKE TLC555% AND elem.package = part.package AND elem.process = reflow; listing all the known footprints of all known packages for parts starting with TLC555, that are good for reflow soldering. The real tables will be somewhat more complicated - it's just to give an idea. The DB avoids all the hassle with file parsing, inventing file formats and in-memory datastructures because all this is done by the server. All one needs is a simple list to receive the answer. The raw table data can be inserted and retrieved using text files, that's formats are well documented and extremely well tested. For what they do DB-servers are even very fast. Armin Hello, Armin. Well, I agree that relational DB is better than text files. I suggested temporary solution because I think we need it until anybody will seriously work to create the database. Is there anyone here who has maybe skeleton for it? It could be first variant to work on. Then gEDA users having ready projects could parse their heavy symbols to grow that DB. VZh ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
What I forgot: my personal experience is with PostgreSQL (have it installed under Linux and Windows XP, Windows Server 2003, works excellent). This is what I would use for a shared environment (eg. web-resource). For read only or single user systems sqlite may be useful. However, the table definitions and some methods of filling the tables should work identical with both. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Armin Faltl wrote: Hello Vladimir, the point in not using a text file format for this but a relational database with SQL is not the data storage but the capabilities of the database server. It allows modeling of relations and more important, relational queries. This can look something like: SELECT elem.footprint FROM elem, part WHERE part.name LIKE TLC555% AND elem.package = part.package AND elem.process = reflow; listing all the known footprints of all known packages for parts starting with TLC555, that are good for reflow soldering. The real tables will be somewhat more complicated - it's just to give an idea. The DB avoids all the hassle with file parsing, inventing file formats and in-memory datastructures because all this is done by the server. All one needs is a simple list to receive the answer. The raw table data can be inserted and retrieved using text files, that's formats are well documented and extremely well tested. For what they do DB-servers are even very fast. Armin Hello, Armin. Well, I agree that relational DB is better than text files. I suggested temporary solution because I think we need it until anybody will seriously work to create the database. Is there anyone here who has maybe skeleton for it? It could be first variant to work on. Then gEDA users having ready projects could parse their heavy symbols to grow that DB. VZh ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Hello Vladimir,
the point in not using a text file format for this but a relational database
with SQL is not the data storage but the capabilities of the database
server.
It allows modeling of relations and more important, relational queries.
This can look something like:
SELECT elem.footprint FROM elem, part
WHERE part.name LIKE TLC555% AND elem.package = part.package AND
elem.process = reflow;
listing all the known footprints of all known packages for parts
starting with TLC555,
that are good for reflow soldering.
The real tables will be somewhat more complicated - it's just to give an
idea.
The DB avoids all the hassle with file parsing, inventing file formats
and in-memory datastructures
because all this is done by the server. All one needs is a simple list
to receive the answer.
The raw table data can be inserted and retrieved using text files,
that's formats are well
documented and extremely well tested. For what they do DB-servers are
even very fast.
Armin
Vladimir Zhbanov wrote:
DJ Delorie wrote:
between footprints and its instances on a board and am able to think
of things like SQL-databases providing a clear, yet flexible mapping
between
Perhaps this idea of mine is relevent?
http://www.delorie.com/pcb/component-dbs.html
Hello.
I am newbie here, too.
My suggestion is to make database in text format for gschem, pcb and
probably others. Idea is that central object is real component from
programs point of view. There should be a way for users to choose
components for their symbols (for example for pin mapping) and/or
symbols/footprints for their components. I intentionally use only
general elements and imply initial schematic capture so DB should be
rather light than heavy.
DB format could be simple and it is stuff to discuss. Simple example:
(component_name (pcb_name1 pcb_name2 ...) (gschem_name1
gschem_name1 ...) ...)
or maybe so:
component=component_name {
company=company_name
...
footprint=footprint_name1
footprint=footprint_name2
...
symbol=sym_name1
symbol=sym_name2
...
whatelse=whatelse1
...
}
and so on.
The database could be distributed and all gEDA programs could use it.
For example I'd like to have common gEDA database and my own local
database which contents line (it is just silly example):
...
(7400 (7400-1.sym 7400-2.sym) (DIP14 DIP14N))
...
That way programs could know what symbols user may use for component.
Then instead of symbol selecting in gschem user could select real
component's name ('component=' attribute?) and preferred symbol and
footprint for it. And in pcb he/she could select required component and
then footprints for it only instead of searching footprint firstly in
datasheet and then in pcb library.
All above could be compromiss for disctinct programs of gEDA project
until new better format will be accepted.
And that way distinct databases for different users, sizes, standarts,
locales and so on could be created.
VZh
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
DJ Delorie wrote:
between footprints and its instances on a board and am able to think
of things like SQL-databases providing a clear, yet flexible mapping
between
Perhaps this idea of mine is relevent?
http://www.delorie.com/pcb/component-dbs.html
Hello.
I am newbie here, too.
My suggestion is to make database in text format for gschem, pcb and
probably others. Idea is that central object is real component from
programs point of view. There should be a way for users to choose
components for their symbols (for example for pin mapping) and/or
symbols/footprints for their components. I intentionally use only
general elements and imply initial schematic capture so DB should be
rather light than heavy.
DB format could be simple and it is stuff to discuss. Simple example:
(component_name (pcb_name1 pcb_name2 ...) (gschem_name1
gschem_name1 ...) ...)
or maybe so:
component=component_name {
company=company_name
...
footprint=footprint_name1
footprint=footprint_name2
...
symbol=sym_name1
symbol=sym_name2
...
whatelse=whatelse1
...
}
and so on.
The database could be distributed and all gEDA programs could use it.
For example I'd like to have common gEDA database and my own local
database which contents line (it is just silly example):
...
(7400 (7400-1.sym 7400-2.sym) (DIP14 DIP14N))
...
That way programs could know what symbols user may use for component.
Then instead of symbol selecting in gschem user could select real
component's name ('component=' attribute?) and preferred symbol and
footprint for it. And in pcb he/she could select required component and
then footprints for it only instead of searching footprint firstly in
datasheet and then in pcb library.
All above could be compromiss for disctinct programs of gEDA project
until new better format will be accepted.
And that way distinct databases for different users, sizes, standarts,
locales and so on could be created.
VZh
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Well like everyone else I have my own crazy way of creating symbols as
I go
along. What I do, is for each part I create a sort of heavy symbol for
that
particular part in its own directory.
What I'd love to see is some sort of wiki of such heavy parts. Each
one could
have mouser part number or whatever. Of course this would cover only a
tiny
fraction of available parts at first, but it might get useful fast: the
most popular
or commonly used parts would get added first. When prototyping you
could
look for a part with a heavy gEDA symbol first.
Even once you have a system for doing it its still a time-consuming
pain
dealing with symbols and footprints all the time.
Britton
On Wed, Apr 21, 2010 at 2:08 PM, Vladimir Zhbanov
[1]vzhba...@gmail.com wrote:
DJ Delorie wrote:
between footprints and its instances on a board and am able to
think
of things like SQL-databases providing a clear, yet flexible
mapping
between
Perhaps this idea of mine is relevent?
[2]http://www.delorie.com/pcb/component-dbs.html
Hello.
I am newbie here, too.
My suggestion is to make database in text format for gschem, pcb and
probably others. Idea is that central object is real component from
programs point of view. There should be a way for users to choose
components for their symbols (for example for pin mapping) and/or
symbols/footprints for their components. I intentionally use only
general elements and imply initial schematic capture so DB should be
rather light than heavy.
DB format could be simple and it is stuff to discuss. Simple
example:
(component_name (pcb_name1 pcb_name2 ...) (gschem_name1
gschem_name1 ...) ...)
or maybe so:
component=component_name {
company=company_name
...
footprint=footprint_name1
footprint=footprint_name2
...
symbol=sym_name1
symbol=sym_name2
...
whatelse=whatelse1
...
}
and so on.
The database could be distributed and all gEDA programs could use
it.
For example I'd like to have common gEDA database and my own local
database which contents line (it is just silly example):
...
(7400 (7400-1.sym 7400-2.sym) (DIP14 DIP14N))
...
That way programs could know what symbols user may use for
component.
Then instead of symbol selecting in gschem user could select real
component's name ('component=' attribute?) and preferred symbol and
footprint for it. And in pcb he/she could select required component
and
then footprints for it only instead of searching footprint firstly
in
datasheet and then in pcb library.
All above could be compromiss for disctinct programs of gEDA project
until new better format will be accepted.
And that way distinct databases for different users, sizes,
standarts,
locales and so on could be created.
VZh
___
geda-user mailing list
[3]geda-u...@moria.seul.org
[4]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
References
1. mailto:vzhba...@gmail.com
2. http://www.delorie.com/pcb/component-dbs.html
3. mailto:geda-user@moria.seul.org
4. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sun, 2010-04-18 at 22:52 +0200, Armin Faltl wrote: Hi, keeping to my promisse, I came up with a skeleton in pseudo-html [...] p bCAVEAT:/b/br If the schematic has to be converted to a board file (.pcb) for use with 'pcb', the value of the ref_des attribute in gschem-symbols must end in a digit ([0-9] - [1-9]?)! /p Maybe someone with write access can add this to section refdes in http://www.geda.seul.org/wiki/geda:glossary Of course, we should try to find the exact reason why refdes like CF or RF without digit may give problems for PCB netlist. Armin, have you tried the suggestion of DJ: ste...@amd64x2 ~/armin $ gsch2pcb project.txt Please try File-Import schematic in the latest PCB, it should work (and needs more testing! :) I can not do this currently, because I am still using 2009 snapshot of PCB shipped with Gentoo-Linux. Best regards Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Stefan Salewski wrote: Armin, have you tried the suggestion of DJ: ste...@amd64x2 ~/armin $ gsch2pcb project.txt Please try File-Import schematic in the latest PCB, it should work (and needs more testing! :) I can not do this currently, because I am still using 2009 snapshot of PCB shipped with Gentoo-Linux. In the next few days I have to try catch up with schedule - this is not a hobby project but work for a customer. Once I got a reasonable board layout, I'll have a look at the svn latest version. Armin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Hi, keeping to my promisse, I came up with a skeleton in pseudo-html (lacks some markup for readability as text) on identifiers and names. It contains the information I learned in the last week(s) and, if fully filled with authoritative information could form the chapter on identifiers in gEDA-interfaces in a gEDA handbook. Best Regards, Armin P.S.: I'm a big fan of good offline documentation. A downloadable set of HTML-pages like e.g. PostgreSQL has it is one of my favourites. Armin Faltl wrote: OMG, it works! Thanks Stefan for all the help. Now the weekend has started. I'll start a Naming conventions and restrictions page to describe this and put on the wiki. In the long run, this should be fixed in the parser(s) though. Best Regards, Armin h2Conventions and Limitations on Identifiers in gEDA/h2 p To give a definition, an identifier is a string entity, that servers as attribute or value or name assigned to an object alone or in combination with other identifiers to describe it in a given context. Examples are symbol attributes and their respective values and file-names. /p h3Composition of an Identifier/h3 p As any string an identifiers is composed of characters with the distinction, that while a string may contain any representable character in an alphabet, an identifier must use a reduced set of characters and in some cases additional restrictions exist, on the relative position of certain characters in the identifier. This serves the purpose, to reserve characters outside the set allowed for identifiers for other syntactic purposes than naming. /p p The different interfaces in gEDA without exception use identifiers - however, as of now the allowed charset and some other restrictions are not the same for every interface, so the interfaces themselves are listed here with detailed description of each of them later on: ul lifile names of several categories/li lisymbol names in schematics in gschem/li lisymbol- and other attributes in schematics/li livalues of attributes in schematics/li /ul /p p To actually note the character sets, the syntax of Perl regular expressions is used. /p h4file names of several categories/h4 h5Schematics/h5 p All valid filename-prefixes of the underlying operating system are allowed. The Suffix is generally '.sch' /p h5Footprint files of newlib/h5 p The suffix for footprint files is generally '.fp'.br !-- fill in lengthy explanation here, how/why fp's with no suffix at all... -- While it is possible to use any prefix allowed by the OS, it is unwise to use '-' (dash) and ' ' (blank) since problems with these have been experienced occasionally. /p h4symbol names in schematics in gschem/h4 p !-- here an indication of what versions of gschem this pertains to is due -- The allowed characters in a symbol name are: [-_.+a-zA-Z0-9] -- this is a guess and by no means authoritative Assumed restrictions by me, Armin: ul limust not end in a '-', since this is used for backups/li limaximal length = N ???/li lion MS-Windows case sensitive names may be a problem/li /ul !-- (- ah yes, these backup files, how they are named is a mess as well - never saw #whatever.some# before ;-) -- This a hrefconvention on naming/a shall help the understanding and exchange of symbols. /p h4Symbol- and other Attributes in Schematics/h4 h4Values of Attributes in Schematics/h4 p bCAVEAT:/b/br If the schematic has to be converted to a board file (.pcb) for use with 'pcb', the value of the ref_des attribute in gschem-symbols must end in a digit ([0-9] - [1-9]?)! /p ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Not because of the bugs I ran into but since choosing a footprint is a difficult process in it self I was longing for a footprint browser. The easiest place to start a clean implementation may be gattrib, that I found conventient to duplicate footprint choices, once one has been assigned gschem. However, the best overview of what is what and therefore choose the right footprint is probably gschem. With gschem open, gattrib should work however, if one remembers, that gschem is in read only then. The problem could be split out of gschem, if it were better supported, to assign a physical part to the symbol. This will probably help other tools too, since e.g. a Spice model is tied to a part, not to a bunch of lines with pins (symbol). I first thought device were the thing to use, but in the standard library it's occupied by names like CAPACITOR_POLARIZED which says noting about rated voltage or ESR. Any ideas? Just my 2 cents Matthew Wilkins wrote: It seems like there is room to add a footprint selector utility that would interface between gschem/gattrib and PCB without impacting non-PCB users in any way. In fact if PCB had an HID where it just starts up as a footprint browser and nothing else, you could use PCB itself to assign footprints to symbols from within gschem or gattrib. An option in the gschem config file could allow users to define a command line to start PCB in that mode, and PCB would output the selected footprint attribute value before exiting. Users of other workflows might be able to use a similar type of browser utility to work with other types of libraries -- gnucap models? verilog models? I don't know if that would be useful or not... Anyway, the point is that this type of feature can be added and could be be completely invisible to other workflows, unless they want to use it. --- On Fri, 4/16/10, DJ Delorie d...@delorie.com wrote: From: DJ Delorie d...@delorie.com Subject: Re: gEDA-user: Matching footprints with symbols To: gEDA user mailing list geda-user@moria.seul.org Received: Friday, April 16, 2010, 6:16 PM Perhaps the shortcoming is in your expectations. I think that (1) our tools are mature enough that users should expect *some* sort of seamless integration and co-operation between them, and (2) we're mature enough to not have to insult our users when our software acts in an unexpected way. The two projects are able to work together *because* they were intentionally designed with clean interfaces, Irrelevent. Having clean interfaces doesn't preclude using those interfaces in a seamless manner, giving the impression of integration. One thing that sows confusion here is that footprint has different meanings Hence the Terminology chaper in the Getting Started guide, which defines what PCB means by footprint: ``A footprint is the pattern on a circuit board to which your parts are attached. This includes all copper, silk, solder mask, and paste information. In other EDA programs, this may be referred to as a land pattern. Footprint sometimes is used to refer to a footprint file. Footprint refers to the pattern; element refers to the instance. For example, your layout might have four elements that use one footprint.'' If you're talking about PCB, please stick with PCB's meanings of the terms. And some design flows don't have footprints (VLSI, simulation, symbolic analysis, ...), although perhaps the hydraulic design process recently discussed here has something analogous ;-) And some programs aren't EDA programs, but that doesn't help with his problem. Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? Please stop trying to push your personal flow onto others :-) Despite you pushing your personal way of doing things (very vocally, I might add), a clear majority (not some) of the geda users DO want a simple schematic - pcb flow that's well integrated and easy to use. Your personal choice is *not it*. Yes, we want to make your flow *possible*, but we really need to make the dumbed-down environment easy to use and streamlined, because that's what most people want. The commercial package owners have a strong incentive to restrict the flow to tools they control, and make it easy to get sucked into their environments. They have little incentive to give you paths to flexibility or higher productivity once you're caught. Flexibility and ease of use should not preclude each other. ___ geda-user mailing list [1]geda-u...@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. file
Re: gEDA-user: Matching footprints with symbols
On Sat, 2010-04-17 at 01:48 +0200, Stefan Salewski wrote: On Sat, 2010-04-17 at 01:15 +0200, Armin Faltl wrote: use ;-) Did anyone try my schematic posted in http://www.seul.org/pipermail/geda-user/2010-April/046716.html - is the problem reproducable? I missed your problem, sorry. One remark: You used the minus sign - in your footprint names. This can give trouble in rare cases due to m4 macro expansion. You may try renaming the footprint files, underscore character _ should work fine. OK, here are the results of closer inspection: I put your files in directory armin: ste...@amd64x2 ~/armin $ ls -1 Hauptplatine_v1.pcb Hauptplatine_v1.sch cap_2.5-5x11-hor.fp cap_3.5-8x11-hor.fp capr_508.fp coil_manual_R16.fp gafrc irf7413-2.sym ltc1625-1.sym project.txt ste...@amd64x2 ~/armin $ To make the symbols in this directory visible to gschem and friends we need this line in gafrc file: ste...@amd64x2 ~/armin $ cat gafrc (component-library .) And we may need the elements-dir . to show gsch2pcb that we have footprints in current directory. (Of course we should use dedicated directories for symbols and footprints later...) ste...@amd64x2 ~/armin $ cat project.txt schematics Hauptplatine_v1.sch output-name Hauptplatine_v1 elements-dir . ste...@amd64x2 ~/armin $ gsch2pcb project.txt = gsch2pcb backend configuration: Variables which may be changed in gafrc: gsch2pcb:pcb-m4-command:/usr/bin/m4 gsch2pcb:pcb-m4-dir:/usr/share/pcb/m4 gsch2pcb:pcb-m4-confdir:/etc/pcb gsch2pcb:pcb-m4-path: /usr/share/pcb/m4 /etc/pcb $HOME/.pcb . gsch2pcb:m4-command-line: /usr/bin/m4 -d -I/usr/share/pcb/m4 -I/etc/pcb -I$HOME/.pcb -I. /usr/share/pcb/m4/common.m4 - Hauptplatine_v1.new.pcb --- Variables which may be changed in the project file: --- gsch2pcb:use-m4:yes = Using the m4 processor for pcb footprints Rf: can't find PCB element for footprint RES-1016-630-240.fp (value=4.7R) So device Rf will not be in the layout. R1: can't find PCB element for footprint RES-1016-630-240.fp (value=3.92k_1%) So device R1 will not be in the layout. R2: can't find PCB element for footprint RES-1016-630-240.fp (value=35.7k_1%) So device R2 will not be in the layout. C_Vcc: can't find PCB element for footprint CAPPR-200P-500D-1100L-50d__Nichicon (value=4.7u) So device C_Vcc will not be in the layout. Db: can't find PCB element for footprint DO-41.fp (value=unknown) So device Db will not be in the layout. -- Done processing. Work performed: 5 file elements and 3 m4 elements added to Hauptplatine_v1.new.pcb. 5 elements could not be found. So Hauptplatine_v1.new.pcb is incomplete. Next steps: 1. Run pcb on your file Hauptplatine_v1.pcb. 2. From within PCB, select File - Load layout data to paste buffer and select Hauptplatine_v1.new.pcb to load the new footprints into your existing layout. 3. From within PCB, select File - Load netlist file and select Hauptplatine_v1.net to load the updated netlist. 4. From within PCB, enter :ExecuteFile(Hauptplatine_v1.cmd) to update the pin names of all footprints. ste...@amd64x2 ~/armin $ ste...@amd64x2 ~/armin $ locate -i RES-1016-630 ste...@amd64x2 ~/armin $ Seems that footptints files are missing on my box, so it is difficult to do further testing. Maybe this already helps. You may try including this line skip-m4 in your project.txt file to ignore m4 files and problems with minus sign in footprint file names. This works, because recent PCB program has copies of all old m4 footprints in newlib format. But it works not perfect, there is some trouble with naming of footprint files. So it may be better to rename your files, replacing the -. Best regards Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sat, 2010-04-17 at 11:57 +0200, Stefan Salewski wrote: You may try including this line skip-m4 in your project.txt file to ignore m4 files and problems with minus sign in footprint file names. This works, because recent PCB program has copies of all old m4 footprints in newlib format. But it works not perfect, there is some trouble with naming of footprint files. So it may be better to rename your files, replacing the -. Ahh -- in your schematic you have footprint names like footprint=RADIAL_CAN 200 with spaces in name, I think this is calling the m4 macro processor. So skip-m4 will not work! But at the same time you are using pcb-symbols-jcl_2008-4-25 and your own containing the problematic minus sign in file name. I think I have to rename all of them, including John Luciani's. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sat, 2010-04-17 at 12:37 +0200, Stefan Salewski wrote: I think I have to rename all of them, including John Luciani's. You have components in your schematic named Rf and Cf without numbers. These seems to have no connection in the netlist. The missing number in refdes seems to be a problem. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Sat, 2010-04-17 at 13:10 +0200, Stefan Salewski wrote: On Sat, 2010-04-17 at 12:37 +0200, Stefan Salewski wrote: I think I have to rename all of them, including John Luciani's. You have components in your schematic named Rf and Cf without numbers. These seems to have no connection in the netlist. The missing number in refdes seems to be a problem. OK, seems to be all fixed now, see http://www.ssalewski.de/tmp/armin20100417.tar refdes without a digit at the end of the name seems to be indeed a big problem, I am not sure if this is stated at a prominent location in the gEDA/PCB documentation? Minus signs in footprint names can be a problem, this should be well known for people reading this list. But I do not know if this was indeed a problem for your current design, I am too lazy to rename all back to minus signs now. Best regards Stefan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Hi, It would be nice to have a revert or reload file function in the gattrib pulldown menu and/or have keystroke. With said feature one would be able to swap more easily between gschem and gattrib when a lot of attributes need to be set/changed (of course updating the file in the process). Just my EUR 0.02 Kind regards, Bert Timmerman. -Original Message- From: geda-user-boun...@moria.seul.org [mailto:geda-user-boun...@moria.seul.org] On Behalf Of Armin Faltl Sent: Saturday, April 17, 2010 11:57 AM To: gEDA user mailing list Subject: Re: gEDA-user: Matching footprints with symbols Not because of the bugs I ran into but since choosing a footprint is a difficult process in it self I was longing for a footprint browser. The easiest place to start a clean implementation may be gattrib, that I found conventient to duplicate footprint choices, once one has been assigned gschem. However, the best overview of what is what and therefore choose the right footprint is probably gschem. With gschem open, gattrib should work however, if one remembers, that gschem is in read only then. The problem could be split out of gschem, if it were better supported, to assign a physical part to the symbol. This will probably help other tools too, since e.g. a Spice model is tied to a part, not to a bunch of lines with pins (symbol). I first thought device were the thing to use, but in the standard library it's occupied by names like CAPACITOR_POLARIZED which says noting about rated voltage or ESR. Any ideas? Just my 2 cents Matthew Wilkins wrote: It seems like there is room to add a footprint selector utility that would interface between gschem/gattrib and PCB without impacting non-PCB users in any way. In fact if PCB had an HID where it just starts up as a footprint browser and nothing else, you could use PCB itself to assign footprints to symbols from within gschem or gattrib. An option in the gschem config file could allow users to define a command line to start PCB in that mode, and PCB would output the selected footprint attribute value before exiting. Users of other workflows might be able to use a similar type of browser utility to work with other types of libraries -- gnucap models? verilog models? I don't know if that would be useful or not... Anyway, the point is that this type of feature can be added and could be be completely invisible to other workflows, unless they want to use it. --- On Fri, 4/16/10, DJ Delorie d...@delorie.com wrote: From: DJ Delorie d...@delorie.com Subject: Re: gEDA-user: Matching footprints with symbols To: gEDA user mailing list geda-user@moria.seul.org Received: Friday, April 16, 2010, 6:16 PM Perhaps the shortcoming is in your expectations. I think that (1) our tools are mature enough that users should expect *some* sort of seamless integration and co-operation between them, and (2) we're mature enough to not have to insult our users when our software acts in an unexpected way. The two projects are able to work together *because* they were intentionally designed with clean interfaces, Irrelevent. Having clean interfaces doesn't preclude using those interfaces in a seamless manner, giving the impression of integration. One thing that sows confusion here is that footprint has different meanings Hence the Terminology chaper in the Getting Started guide, which defines what PCB means by footprint: ``A footprint is the pattern on a circuit board to which your parts are attached. This includes all copper, silk, solder mask, and paste information. In other EDA programs, this may be referred to as a land pattern. Footprint sometimes is used to refer to a footprint file. Footprint refers to the pattern; element refers to the instance. For example, your layout might have four elements that use one footprint.'' If you're talking about PCB, please stick with PCB's meanings of the terms. And some design flows don't have footprints (VLSI, simulation, symbolic analysis, ...), although perhaps the hydraulic design process recently discussed here has something analogous ;-) And some programs aren't EDA programs, but that doesn't help with his problem. Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? Please stop trying to push your personal flow onto others :-) Despite you pushing your personal way of doing things (very vocally, I might add), a clear majority (not some) of the geda users DO want a simple schematic
Re: gEDA-user: Matching footprints with symbols
The 'RADIAL_CAN 200' I used to replace Luciani-footprints (I don't blame him but the parser), after this proved non-working. It is interesting to note, that in the file Hauptplatine_v1.new.pcb generated by gsch2pcb, they translate to RADIAL_CAN-200 in the Element-definition. Maybe it is somewhere, but an authoritative definition of what characters are allowed in identifiers seems to be badly lacking. This definition must hold valid for the entire gEDA suite. Otherwise an integration of any kind is doomed to fail. Looking at this I recall a statement about file-format evolvement: ...the file format must stay backwards compatible. - I dare to negate this: All the files I encountered but the netlist have a version specifier as their 1st line. It is sufficient to adhere to this feature. All other characteristics can be changed and some should. A good idea to me is to adherere to the JSON syntax definition for future exchange formats. http://www.json.org/ For netlists one might consider ref_des:N instead of ref_des-N. Regards, Armin Stefan Salewski wrote: On Sat, 2010-04-17 at 11:57 +0200, Stefan Salewski wrote: You may try including this line skip-m4 in your project.txt file to ignore m4 files and problems with minus sign in footprint file names. This works, because recent PCB program has copies of all old m4 footprints in newlib format. But it works not perfect, there is some trouble with naming of footprint files. So it may be better to rename your files, replacing the -. Ahh -- in your schematic you have footprint names like footprint=RADIAL_CAN 200 with spaces in name, I think this is calling the m4 macro processor. So skip-m4 will not work! But at the same time you are using pcb-symbols-jcl_2008-4-25 and your own containing the problematic minus sign in file name. I think I have to rename all of them, including John Luciani's. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
OMG, it works! Thanks Stefan for all the help. Now the weekend has started. I'll start a Naming conventions and restrictions page to describe this and put on the wiki. In the long run, this should be fixed in the parser(s) though. Best Regards, Armin Stefan Salewski wrote: On Sat, 2010-04-17 at 13:10 +0200, Stefan Salewski wrote: On Sat, 2010-04-17 at 12:37 +0200, Stefan Salewski wrote: I think I have to rename all of them, including John Luciani's. You have components in your schematic named Rf and Cf without numbers. These seems to have no connection in the netlist. The missing number in refdes seems to be a problem. OK, seems to be all fixed now, see http://www.ssalewski.de/tmp/armin20100417.tar refdes without a digit at the end of the name seems to be indeed a big problem, I am not sure if this is stated at a prominent location in the gEDA/PCB documentation? Minus signs in footprint names can be a problem, this should be well known for people reading this list. But I do not know if this was indeed a problem for your current design, I am too lazy to rename all back to minus signs now. Best regards Stefan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
ste...@amd64x2 ~/armin $ gsch2pcb project.txt Please try File-Import schematic in the latest PCB, it should work (and needs more testing! :) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 10:44 PM, Matthew Wilkins wrote: It seems like there is room to add a footprint selector utility that would interface between gschem/gattrib and PCB without impacting non-PCB users in any way. In fact if PCB had an HID where it just starts up as a footprint browser and nothing else, you could use PCB itself to assign footprints to symbols from within gschem or gattrib. An option in the gschem config file could allow users to define a command line to start PCB in that mode, and PCB would output the selected footprint attribute value before exiting. Users of other workflows might be able to use a similar type of browser utility to work with other types of libraries -- gnucap models? verilog models? I don't know if that would be useful or not... Anyway, the point is that this type of feature can be added and could be be completely invisible to other workflows, unless they want to use it. Completely invisible? No! 1. Any feature must be documented. Every addition to the documentation adds to the fog hiding the the other parts of the documentation. One of the advantages of a clean, simple, well-factored, modular approach is that it simplifies the documentation. 2. Any feature can be misconfigured. 3. Any feature can be misunderstood. In commercial software, there's tremendous pressure to add features, with the result that bloated, low productivity tools are the norm. A free tool need not follow that path. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
No, I stand by it - zero impact.As far as I can see, all of the required features are are already existing in gschem, so there really wouldn't be any feature bloat. This would be something that could be added on by PCB users with a few edits to the gschemrc files. --- On Sat, 4/17/10, John Doty j...@noqsi.com wrote: From: John Doty j...@noqsi.com Subject: Re: gEDA-user: Matching footprints with symbols To: gEDA user mailing list geda-user@moria.seul.org Received: Saturday, April 17, 2010, 1:10 PM On Apr 16, 2010, at 10:44 PM, Matthew Wilkins wrote: It seems like there is room to add a footprint selector utility that would interface between gschem/gattrib and PCB without impacting non-PCB users in any way. In fact if PCB had an HID where it just starts up as a footprint browser and nothing else, you could use PCB itself to assign footprints to symbols from within gschem or gattrib. An option in the gschem config file could allow users to define a command line to start PCB in that mode, and PCB would output the selected footprint attribute value before exiting. Users of other workflows might be able to use a similar type of browser utility to work with other types of libraries -- gnucap models? verilog models? I don't know if that would be useful or not... Anyway, the point is that this type of feature can be added and could be be completely invisible to other workflows, unless they want to use it. Completely invisible? No! 1. Any feature must be documented. Every addition to the documentation adds to the fog hiding the the other parts of the documentation. One of the advantages of a clean, simple, well-factored, modular approach is that it simplifies the documentation. 2. Any feature can be misconfigured. 3. Any feature can be misunderstood. In commercial software, there's tremendous pressure to add features, with the result that bloated, low productivity tools are the norm. A free tool need not follow that path. John Doty Noqsi Aerospace, Ltd. [1]http://www.noqsi.com/ [2]...@noqsi.com ___ geda-user mailing list [3]geda-u...@moria.seul.org [4]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. http://www.noqsi.com/ 2. file://localhost/mc/compose?to=...@noqsi.com 3. file://localhost/mc/compose?to=geda-u...@moria.seul.org 4. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 8:47 PM, kai-martin knaak wrote: John Doty wrote: Please stop trying to push your personal flow onto others :-) Which one? your makefile approach. Heck, I don't even push that one on myself. For a small project, who needs it? But for a big project, there's no effective substitute. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Thu, 15 Apr 2010 10:23:08 -0500, John Griessen wrote: Here is something you might like -- I fixed this up the other day: http://cottagematic.com/examples/ It's a project skeleton, (plus contents), that lets you access the symbol and footprint libraries contained in it without changing your global settings. My new_geda_project.sh script is bit more low key. When given a project name, it creates a simple directory structure and populates it with some config files (gafrc, attribs). In addition, it copies a documentation template in lyx format to the directory. The script is available at my section of gedasymbols.org: http://www.gedasymbols.org/user/kai_martin_knaak/ ---)kaimartin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
No, that's not what I'm talking about. Footprints depend on the layout tool: gschem is properly agnostic about what layout tool you're using. John Doty Noqsi Aerospace, Ltd. [1]http://www.noqsi.com/ [2]...@noqsi.com So that means the shortcoming is with gchs2cpb? We need a better way of stitching two disparate (and intentionally agnostic) tools that newcomers wish to use as if they were an application suite. We need some way for gsch2pcb to stop at each undefined or unmatched footprint, and since we are running gsch2pcb, we know that the origin of the item is a symbol in gschem, so the symbol can be listed, described, tabulated, or displayed, and then a file browsing window, dialog box, command line menu would open up to go searching to find a matching footprint for that symbol, do some basic reality checks on the pin numbers/names/attributes and possibly either allow the user to fix problems in the symbol or footprint and save the modified version in the project directory, or allow the user to keep looking for a better match. This would be easiest if done in a GUI like gschem and pcb, but possible even for a command line only interface. Although matching up pins and pads in two text listings of symbol and footprint attributes would be difficult. By moving the 'repair' process to gsch2pcb, it would allow gschem and pcb to remain completely agnostic of each other, although to me that sounds more like slightly incompatible with each other. On the other hand, I have never used Spice or any other the other second programs (backends?) that gschem is expected to feed. It may be that with that wider perspective I would be able to see clearly why you want gschem and pcb to remain disjoint. On the other hand, if the interface and conversion programs and scripts between all the tools was more complete, intuitive and foolproof, then the entire package of tools could be combined under a single IDE and act like a unified suite of tools, like I expect most of the commercial packages work. Mike References 1. http://www.noqsi.com/ 2. mailto:j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 10:49 AM, Mike Bushroe wrote: No, that's not what I'm talking about. Footprints depend on the layout tool: gschem is properly agnostic about what layout tool you're using. John Doty Noqsi Aerospace, Ltd. [1]http://www.noqsi.com/ [2]...@noqsi.com So that means the shortcoming is with gchs2cpb? Perhaps the shortcoming is in your expectations. We need a better way of stitching two disparate (and intentionally agnostic) tools that newcomers wish to use as if they were an application suite. The two projects are able to work together *because* they were intentionally designed with clean interfaces, and no unnecessary entanglements. You propose to throw away the very virtue that made the partnership possible in the first place. Some of us want to keep the tools open to other partnerships. We need some way for gsch2pcb to stop at each undefined or unmatched footprint, and since we are running gsch2pcb, we know that the origin of the item is a symbol in gschem, so the symbol can be listed, described, tabulated, or displayed, and then a file browsing window, dialog box, command line menu would open up to go searching to find a matching footprint for that symbol, do some basic reality checks on the pin numbers/names/attributes and possibly either allow the user to fix problems in the symbol or footprint and save the modified version in the project directory, or allow the user to keep looking for a better match. This would be easiest if done in a GUI like gschem and pcb, but possible even for a command line only interface. Although matching up pins and pads in two text listings of symbol and footprint attributes would be difficult. One thing that sows confusion here is that footprint has different meanings to the person choosing the part and to the person laying out the board. The pattern of pins on isn't the same thing as the pattern of pads on the board, and there isn't a one-to-one relationship. Different manufacturing processes need different pad patterns for the same physical part. And some design flows don't have footprints (VLSI, simulation, symbolic analysis, ...), although perhaps the hydraulic design process recently discussed here has something analogous ;-) By moving the 'repair' process to gsch2pcb, it would allow gschem and pcb to remain completely agnostic of each other, although to me that sounds more like slightly incompatible with each other. On the other hand, I have never used Spice or any other the other second programs (backends?) that gschem is expected to feed. It may be that with that wider perspective I would be able to see clearly why you want gschem and pcb to remain disjoint. On the other hand, if the interface and conversion programs and scripts between all the tools was more complete, intuitive and foolproof, then the entire package of tools could be combined under a single IDE Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? and act like a unified suite of tools, like I expect most of the commercial packages work. The commercial package owners have a strong incentive to restrict the flow to tools they control, and make it easy to get sucked into their environments. They have little incentive to give you paths to flexibility or higher productivity once you're caught. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Perhaps the shortcoming is in your expectations. I think that (1) our tools are mature enough that users should expect *some* sort of seamless integration and co-operation between them, and (2) we're mature enough to not have to insult our users when our software acts in an unexpected way. The two projects are able to work together *because* they were intentionally designed with clean interfaces, Irrelevent. Having clean interfaces doesn't preclude using those interfaces in a seamless manner, giving the impression of integration. One thing that sows confusion here is that footprint has different meanings Hence the Terminology chaper in the Getting Started guide, which defines what PCB means by footprint: ``A footprint is the pattern on a circuit board to which your parts are attached. This includes all copper, silk, solder mask, and paste information. In other EDA programs, this may be referred to as a land pattern. Footprint sometimes is used to refer to a footprint file. Footprint refers to the pattern; element refers to the instance. For example, your layout might have four elements that use one footprint.'' If you're talking about PCB, please stick with PCB's meanings of the terms. And some design flows don't have footprints (VLSI, simulation, symbolic analysis, ...), although perhaps the hydraulic design process recently discussed here has something analogous ;-) And some programs aren't EDA programs, but that doesn't help with his problem. Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? Please stop trying to push your personal flow onto others :-) Despite you pushing your personal way of doing things (very vocally, I might add), a clear majority (not some) of the geda users DO want a simple schematic - pcb flow that's well integrated and easy to use. Your personal choice is *not it*. Yes, we want to make your flow *possible*, but we really need to make the dumbed-down environment easy to use and streamlined, because that's what most people want. The commercial package owners have a strong incentive to restrict the flow to tools they control, and make it easy to get sucked into their environments. They have little incentive to give you paths to flexibility or higher productivity once you're caught. Flexibility and ease of use should not preclude each other. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 4:16 PM, DJ Delorie wrote: Please stop trying to push your personal flow onto others :-) Which one? John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 4:16 PM, DJ Delorie wrote: Flexibility and ease of use should not preclude each other. But they generally do. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
The two projects are able to work together *because* they were intentionally designed with clean interfaces, Irrelevent. Having clean interfaces doesn't preclude using those interfaces in a seamless manner, giving the impression of integration. While I'm fully ok with a script doing the integration (that can very easily be invoked by a wrapper providing a button aka IDE) I want to second this and describe how I think the internal working may be influenced: *) as it is deterministic, that attachment of a footprint with non-matching pin/pad-numbers to a given symbol - that is last seen by the converter if I understand it right - will cause trouble, a clean converter will reject such combinations and list the - ref-des - symbol(-file) - path the symbol was found in - footprint(-file) - path the footprint was found in of the offending aggregate per default. If this causes laughter in some corners, forgive me, I'm not aware of all the flags the converters might have and man gsch2pcb produces nothing on my system. [snip] Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? While I see fit and like scripts my fight with gEDA the last 2 weeks can by no means be described as productive - I used Eagle before, but as this was hobby and would be illegal with what I (try to) do now. Believe me, I fully understand the difference between footprints and its instances on a board and am able to think of things like SQL-databases providing a clear, yet flexible mapping between - symbols - physical packages - vendor part numbers - manufacturing process - board characteristics (1 ounce, 2 ounce, FR2, FR4, ...) - HF electrical charateristics, thermal,... It would however be very convenient for me, if I can be sure, that missing pins in the ratsnest tool are not due to an incompatible choice of footprint for a symbol. Armin Faltl ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 16, 2010, at 4:16 PM, DJ Delorie wrote: Hence the Terminology chaper in the Getting Started guide, which defines what PCB means by footprint: ``A footprint is the pattern on a circuit board to which your parts are attached. This includes all copper, silk, solder mask, and paste information. In other EDA programs, this may be referred to as a land pattern. Footprint sometimes is used to refer to a footprint file. Footprint refers to the pattern; element refers to the instance. For example, your layout might have four elements that use one footprint.'' If you're talking about PCB, please stick with PCB's meanings of the terms. I don't use pcb, although I design circuits that will be implemented on PCB's ;-) I do use gschem, and it's much less clear from that point of view what footprint means, although in the footprint naming conventions document that we used to have it was clear that it referred to the part, not the board. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Flexibility and ease of use should not preclude each other. But they generally do. On the commandline options are for flexibility, defaults are for ease of use ;-) Did anyone try my schematic posted in http://www.seul.org/pipermail/geda-user/2010-April/046716.html - is the problem reproducable? Dipl. Ing. Armin Faltl Mechatroniker für Maschinen- u. Fertigungstechnik Schlosserei Heinrich Leflergasse 6, A-1220 Wien e-mail: armin.fa...@aon.at mobile: +43 664/547 68 68 phone : +43 1 282 86 38 UID-Nr: ATU-56556122 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
The two projects are able to work together *because* they were intentionally designed with clean interfaces, and no unnecessary entanglements. You propose to throw away the very virtue that made the partnership possible in the first place. Some of us want to keep the tools open to other partnerships. John-- He was proposing no such thing and you know it perfectly well. You don't need to keep making up stuff like this. You have told us all *many* times how important it is that the gEDA suite is made up of independent toolkit programs that have clean interfaces, supporting all kinds of unique workflows. I think that there's a consensus here that this is a genuine strength of the gEDA suite. Yes, we agree with you. We also know that you personally have a special workflow, and *nobody* is trying to take that away from you. So far so good. But, maybe it's time that you face facts: 1.) Some of us think that it's actually okay to use gschem together in a workflow with pcb. 2.) Some of us think that it's okay to add additional, easy-to-use (and yes, integrated) interfaces so long as they don't interfere with existing scriptable command-line operation. I personally think that it's good (in general) to build the gEDA community. Starting people off with an example workflow (e.g., gschem to pcb) may be a good way to get them in the door-- so that they can start to see how they might instead design more unique workflows between the different programs. 3.) You're too late. There is already (more than one) existing integration between gschem and pcb. Fortunately, gsch2pcb is an independent program, so changes to it do not throw away the clean interfaces between the other programs, but instead makes use of it. On the one hand, you seem to value gEDA, its independence between programs, and the fact that anyone can write their own customized scripts to make an efficient custom workflow between the programs that they want to use. However if that's really the case, you should also understand that it's okay if people do exactly that, but with workflows that are different from your own. For example if people want to discuss modifications to gsch2pcb (or other programs that you don't use), the very least that you could do is stay out of it. It's not actually necessary for you to go out of your way to bash them. It gets old pretty quickly; please give it a rest. We mostly agree with you. It would nice if you agreed with you too. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
between footprints and its instances on a board and am able to think of things like SQL-databases providing a clear, yet flexible mapping between Perhaps this idea of mine is relevent? http://www.delorie.com/pcb/component-dbs.html ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Phil Frost wrote: As Linux filesystem developer and convicted wife murderer Hans Rieser wrote: The expressive power of an operating system is NOT proportional to the number of components, but instead is proportional to the number of possible connections between its components. I want to make an open hardware vision system board that uses Cognimem chips or any neural hardware with gEDA tools so bad... John -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
John Doty wrote: Please stop trying to push your personal flow onto others :-) Which one? your makefile approach. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
It seems like there is room to add a footprint selector utility that would interface between gschem/gattrib and PCB without impacting non-PCB users in any way. In fact if PCB had an HID where it just starts up as a footprint browser and nothing else, you could use PCB itself to assign footprints to symbols from within gschem or gattrib. An option in the gschem config file could allow users to define a command line to start PCB in that mode, and PCB would output the selected footprint attribute value before exiting. Users of other workflows might be able to use a similar type of browser utility to work with other types of libraries -- gnucap models? verilog models? I don't know if that would be useful or not... Anyway, the point is that this type of feature can be added and could be be completely invisible to other workflows, unless they want to use it. --- On Fri, 4/16/10, DJ Delorie d...@delorie.com wrote: From: DJ Delorie d...@delorie.com Subject: Re: gEDA-user: Matching footprints with symbols To: gEDA user mailing list geda-user@moria.seul.org Received: Friday, April 16, 2010, 6:16 PM Perhaps the shortcoming is in your expectations. I think that (1) our tools are mature enough that users should expect *some* sort of seamless integration and co-operation between them, and (2) we're mature enough to not have to insult our users when our software acts in an unexpected way. The two projects are able to work together *because* they were intentionally designed with clean interfaces, Irrelevent. Having clean interfaces doesn't preclude using those interfaces in a seamless manner, giving the impression of integration. One thing that sows confusion here is that footprint has different meanings Hence the Terminology chaper in the Getting Started guide, which defines what PCB means by footprint: ``A footprint is the pattern on a circuit board to which your parts are attached. This includes all copper, silk, solder mask, and paste information. In other EDA programs, this may be referred to as a land pattern. Footprint sometimes is used to refer to a footprint file. Footprint refers to the pattern; element refers to the instance. For example, your layout might have four elements that use one footprint.'' If you're talking about PCB, please stick with PCB's meanings of the terms. And some design flows don't have footprints (VLSI, simulation, symbolic analysis, ...), although perhaps the hydraulic design process recently discussed here has something analogous ;-) And some programs aren't EDA programs, but that doesn't help with his problem. Ugh! Yuck! IDE = Inflexible, Dumbed-down Environment. Some prefer that, but shouldn't there remain toolkits for those of us who need flexibility and high productivity automation? Please stop trying to push your personal flow onto others :-) Despite you pushing your personal way of doing things (very vocally, I might add), a clear majority (not some) of the geda users DO want a simple schematic - pcb flow that's well integrated and easy to use. Your personal choice is *not it*. Yes, we want to make your flow *possible*, but we really need to make the dumbed-down environment easy to use and streamlined, because that's what most people want. The commercial package owners have a strong incentive to restrict the flow to tools they control, and make it easy to get sucked into their environments. They have little incentive to give you paths to flexibility or higher productivity once you're caught. Flexibility and ease of use should not preclude each other. ___ geda-user mailing list [1]geda-u...@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user References 1. file://localhost/mc/compose?to=geda-u...@moria.seul.org 2. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
John Doty wrote: I think it's far more important to have the symbol browser import symbols into the *project* (not the schematic) as they are selected, so they can be customized as necessary. And it should pop up an annoying information box reminding the user to check the symbol until the user turns the box off. A GUI way to move symbol files from within gschem and footprints from within pcb would be a welcome feature by me and many. It would enable project dir design method for newbies, and help them check an qualify symbols and footprints. It's still not hard to do with the command line and I often rename generic borrowed symbols and footprints to match. The matching names signify checked good to me. Depending on standard libraries just referenced by a project stops you from having this easy indication of checked good, since you can't change names of standard libraries. John -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Amand Tihon wrote: Please bear with me, I'm just a hobbyist. I've never had to work with a contractor or manufacturer. Ce n'est pas de rien trouble, Amand. Ask away. John -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 14, 2010, at 10:41 AM, Amand Tihon wrote: Hi everyone. I'm new to this list, and a very occasional gschem/pcb user. I make probably one or two small boards per year, single layer. Most of the time using through-hole components because that's what available at my local shop. My question may sound silly or may even have been asked countless times: Yep. And the problem is that we downplay the truth: the library symbols are only starting points, not sensibly used as-is. Are there any official guidelines for naming/numbering pins and pads on symbols and footprints ? Some packages have an obvious numbering like DIP, but what about capacitors, diodes, transistors, etc. ? It could be due to my distribution (Debian), but I always get lost in the symbols and footprints libraries that come with gEDA. Finding the right footprint with correct pin numbering has always been a challenge. Yep. The problem afflicts all EDA systems because there are no universal standards for the physical parts. One even encounters DIP packages with reversed numbers occasionally (Minicircuits). For instance, there are 3 different LED symbols. One in Basic devices, two in Diodes (generic). Two of them have the anode on pin 1, the third one has it on pin 2. When trying to find a footprint for it, there are more than five for each of 3mm and 5mm LEDs. For *none* of them does the silkscreen indicate the position of the anode or cathode. LED3 and LED5 from pcblib/~geda actually present this information in their name/description: (pin 1 is +, 2 is-). In pcblib/~optical, however, the squared pin is named - (in red in preview, still not on the silkscreen). How do you usually handle this ? Copy the symbol file into the project's symbol directory and edit it to match my project's parts and design flow. Might be nice for beginners if the GUI did the copy, although it's trivial from command line. Maybe you are able to remember what footprint will match which symbol, but I don't use gEDA often enough for that. Or do you build your libraries of symbols and footprints that you *know* (or hope) are correct ? Perhaps the state of the SMDs footprints is not that bad ? I'm now slowly building my own libraries of footprints and heavy-wheight symbols, to avoid mismatch between symbols and footprints. Another reason I'm doing it is because I drill the holes by hand whithout any drill-stand: my footprints have large (60 or 80 mil) pins that allow for some imprecision, with 15 mil drill hole to have the drill bit position itself right on spot, thanks to the copper thickness :) The drawback is that those footprints are obviously unusable if I ever need to have a board manufactured. Thanks for your answers. -- Amand Tihon 13C Rue Arsène Matton, 1325 Dion-Valmont, Belgium +32 479 207 743 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Amand Tihon wrote: Hi everyone. It could be due to my distribution (Debian), but I always get lost in the symbols and footprints libraries that come with gEDA. There are even more at gedasymbols.org and luciani.org For *none* of them does the silkscreen indicate the position of the anode or cathode. Or do you build your libraries of symbols and footprints that you *know* (or hope) are correct ? Yes. There has been talk of somehow proofreading symbol/footprint pairs for correct netlisting and good soldering, but it has not evolved into anything very complete -- just what you can find on individual pages of sites above. Perhaps the state of the SMDs footprints is not that bad ? I amusing a plc44 from there. It seems good dimensions. DJ, (and many here probably), prints out pdf of layout and tries out parts for fit on it. I'm now slowly building my own libraries of footprints and heavy-wheight symbols, to avoid mismatch between symbols and footprints. I found parts of a workflow and changed it to suit me that lets you keep local libraries easily. See if you like this: http://cottagematic.com/examples/ With a project directory approach like in that tarball, you could change your local ./pcb.settings file to reference a different subdirectory of footprints with the same names to have a pcb layout with smaller holes for manufacturing. I'm not remembering how the referencing of different footprints works in pcb -- it may be the footprints are sort of embedded and you have to reset that somehow -- needs some reading the pcb manual. Another reason I'm doing it is because I drill the holes by hand whithout any drill-stand: my footprints have large (60 or 80 mil) pins that allow for some imprecision, with 15 mil drill hole to have the drill bit position itself right on spot, thanks to the copper thickness :) The drawback is that those footprints are obviously unusable if I ever need to have a board manufactured. They may be unusable as is, but you can use the pcb command window to change drill sizes of groups of selected pins, vias. Example commands for that: ChangeDrillSize(SelectedObjects, 32, mil ) ChangeSize(SelectedObjects, 62.0, mil ) John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Wed, 14 Apr 2010 18:41:44 +0200, Amand Tihon wrote: It could be due to my distribution (Debian), but I always get lost in the symbols and footprints libraries that come with gEDA. Finding the right footprint with correct pin numbering has always been a challenge. You are not the only one. This is consequence of a number of unresolved issues: 1) Unlike other EDA applications, there is no notion of a package that contains both: symbols and footprints. 2) gschem and pcb are historically distinct. There are strong forces in the developer community that discourage any closer relationship between than the current import-export. 3) There is consensus, that the current library is in poor shape. But there are diverging opinions how a good default library should look like. For instance, there are 3 different LED symbols. One in Basic devices, two in Diodes (generic). Two of them have the anode on pin 1, the third one has it on pin 2. When trying to find a footprint for it, there are more than five for each of 3mm and 5mm LEDs. For *none* of them does the silkscreen indicate the position of the anode or cathode. LED3 and LED5 from pcblib/~geda actually present this information in their name/description: (pin 1 is +, 2 is-). In pcblib/~optical, however, the squared pin is named - (in red in preview, still not on the silkscreen). The default library of gschem is a known weakness. It was already in exactly the same shape in 2005 when I started to work with geda. How do you usually handle this ? I don't use the default lib and rely entirely on my homegrow symbols/ footprints. See my section on gedasymbols.org. Maybe you are able to remember what footprint will match which symbol, but I don't use gEDA often enough for that. No. All my symbols contain a default footprint. One of my favourite feature requests is the ability to give a list of default footprints. Or do you build your libraries of symbols and footprints that you *know* (or hope) are correct ? yes. Perhaps the state of the SMDs footprints is not that bad ? I'm now slowly building my own libraries of footprints and heavy-wheight symbols, to avoid mismatch between symbols and footprints. Please consider uploading them in your own section at gedasymbols.org :-) ---)kaiamrtin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Le mercredi 14 avril 2010 19:18:19, Kai-Martin Knaak a écrit : On Wed, 14 Apr 2010 18:41:44 +0200, Amand Tihon wrote: It could be due to my distribution (Debian), but I always get lost in the symbols and footprints libraries that come with gEDA. Finding the right footprint with correct pin numbering has always been a challenge. You are not the only one. This is consequence of a number of unresolved issues: 1) Unlike other EDA applications, there is no notion of a package that contains both: symbols and footprints. Well, I've never used any other EDA application. I imagine packages could help if well designed, but then there's your point 2). 2) gschem and pcb are historically distinct. There are strong forces in the developer community that discourage any closer relationship between than the current import-export. I think that having common guidelines would keep both projects independant but ease symbols and footprints creation. For instance: - Simple diode: anode is on pin 1. - Polarized capacitor: + is on pin 1. - Default TO-92 footprint is 1-2-3 when looking at the flat side, pins down - etc. Do such guidelines exist ? 3) There is consensus, that the current library is in poor shape. But there are diverging opinions how a good default library should look like. The net result seems to have been the creation of gedasymbols.org: a collection of symbols, sometimes with matching footprints, that you still cannot trust blindly because everyone has his own rules for pins numbering. John Doty said that the libraries shipped with gEDA should be used as starting points. I tend to think that gedasymbols.org makes a much better starting point. The default library of gschem is a known weakness. It was already in exactly the same shape in 2005 when I started to work with geda. Sadly, that matches my feelings about it. I don't use the default lib and rely entirely on my homegrow symbols/ footprints. Does anyone actually use the stock symbols ? All my symbols contain a default footprint. One of my favourite feature requests is the ability to give a list of default footprints. Is that a feature worth working on (I'm a developer, electronics is a hobby) ? Or would such a patch be rejected without hope of being ever integrated ? I'm now slowly building my own libraries of footprints and heavy-wheight symbols, to avoid mismatch between symbols and footprints. Please consider uploading them in your own section at gedasymbols.org :-) I will. Thanks for your answers. -- Amand Tihon 13C Rue Arsène Matton, 1325 Dion-Valmont, Belgium +32 479 207 743 signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 14, 2010, at 10:18 AM, Kai-Martin Knaak wrote: 3) There is consensus, that the current library is in poor shape. But there are diverging opinions how a good default library should look like. And I doubt there will ever be a one size fits all library. The flexibility of the current system is it's strength, you can pretty much always get what you want, or close enough. OTOH, the flexibility of the current system causes no end of confusion to new users. I think that there are probably different libraries for different user communities. I can think of two footprint libraries right off: a) result must be easy to hand solder -- either because the user is a hobbyist or someone who wants to create kits for a hobbyist community where you want good results to come easily, and b) result targets automated manufacturing at low cost, using lots of SMT. And when it comes to symbols, then it gets into religious arguments :) I like symbols that might pass for ANSI compliant. And I split the power/ground/infrastructure into a second block. Either of those ideas can make other people wince. So it gets tangled up in methodology arguments, too. So, in an ideal world, I could see having different communities (Library SIGs) support different libraries. A community/library being defined by a list of design rules and methodology guidelines. Anyway, all that said, I think that is expecting a lot for the gEDA community to form library SIGs around different design rule manifestos. There just aren't enough of us to go around. For the time being we are all Library SIGs of one person each :) -dave ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Le mercredi 14 avril 2010 19:12:59, John Griessen a écrit : They may be unusable as is, but you can use the pcb command window to change drill sizes of groups of selected pins, vias. Example commands for that: ChangeDrillSize(SelectedObjects, 32, mil ) ChangeSize(SelectedObjects, 62.0, mil ) I was about to reply that it wouldn't change the size of my oval pads, but on second thought, it shouldn't be an issue at all. Thanks. -- Amand Tihon 13C Rue Arsène Matton, 1325 Dion-Valmont, Belgium +32 479 207 743 signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Le mercredi 14 avril 2010 20:29:59, Dave N6NZ a écrit : On Apr 14, 2010, at 10:18 AM, Kai-Martin Knaak wrote: 3) There is consensus, that the current library is in poor shape. But there are diverging opinions how a good default library should look like. And I doubt there will ever be a one size fits all library. The flexibility of the current system is it's strength, you can pretty much always get what you want, or close enough. OTOH, the flexibility of the current system causes no end of confusion to new users. I'm certainly not ranting about the symbols/footprints separation here. I understand very well that this flexibility is appreciated. I think that there are probably different libraries for different user communities. I can think of two footprint libraries right off: a) result must be easy to hand solder -- either because the user is a hobbyist or someone who wants to create kits for a hobbyist community where you want good results to come easily, and b) result targets automated manufacturing at low cost, using lots of SMT. The problem (as I see it from my humble point of view) is that the default libraries target none. Hobbyists will have a hard time finding matching footprints, lose time drawing new ones, and end with a board that fails the smoke test because of inconsistent pinout. I learnt it the hard way :) Pros will redraw a good amount of the symbols and footprints anyway, to have them match their SIGs. Anyway, all that said, I think that is expecting a lot for the gEDA community to form library SIGs around different design rule manifestos. There just aren't enough of us to go around. For the time being we are all Library SIGs of one person each :) :) Where I see guidelines could help is not in the design itself but on the properties of the symbols and footprints. If only I could download a footprint for a capacitor and be certain, without even checking, that the pinout would match the one used in the symbol I downloaded from somewhere else! Something like that would help. Currently, I cannot even trust the default library for that. Anyway, thank you for your time. I'll continue to make my own libraries :) -- Amand Tihon 13C Rue Arsène Matton, 1325 Dion-Valmont, Belgium +32 479 207 743 signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 14, 2010, at 12:27 PM, Amand Tihon wrote: I think that having common guidelines would keep both projects independant but ease symbols and footprints creation. For instance: - Simple diode: anode is on pin 1. - Polarized capacitor: + is on pin 1. - Default TO-92 footprint is 1-2-3 when looking at the flat side, pins down - etc. Do such guidelines exist ? No, and they wouldn't work. The layout person is going to want numbers matching their own tool and footprint library. There are no standards here. The technician working on the board is going to want to see pin numbers matching the manufacturer's data sheet, and manufacturers have no common numbering scheme. gEDA can't unilaterally fix these problems. 3) There is consensus, that the current library is in poor shape. But there are diverging opinions how a good default library should look like. The net result seems to have been the creation of gedasymbols.org: a collection of symbols, sometimes with matching footprints, that you still cannot trust blindly because everyone has his own rules for pins numbering. You can *NEVER* trust a library symbol blindly. In any EDA system. Period. Get over it. John Doty said that the libraries shipped with gEDA should be used as starting points. I tend to think that gedasymbols.org makes a much better starting point. The default library of gschem is a known weakness. It was already in exactly the same shape in 2005 when I started to work with geda. Sadly, that matches my feelings about it. Feelings don't matter. It's like complaining that there's no solution for the general quintic equation using radicals. It's a known weakness of algebra, but it's also known to be unfixable, so move on. I don't use the default lib and rely entirely on my homegrow symbols/ footprints. Does anyone actually use the stock symbols ? For a simple project there's nothing wrong with resistor-1.sym. For a more complex project, I generally want some project-specific default attributes like footprint=0603 and spec=1/16W,5%. The customer, layout contractor, and application have an influence here. All my symbols contain a default footprint. One of my favourite feature requests is the ability to give a list of default footprints. Is that a feature worth working on (I'm a developer, electronics is a hobby) ? Or would such a patch be rejected without hope of being ever integrated ? I think it's far more important to have the symbol browser import symbols into the *project* (not the schematic) as they are selected, so they can be customized as necessary. And it should pop up an annoying information box reminding the user to check the symbol until the user turns the box off. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
Le mercredi 14 avril 2010 21:45:24, John Doty a écrit : Do such guidelines exist ? No, and they wouldn't work. The layout person is going to want numbers matching their own tool and footprint library. There are no standards here. The technician working on the board is going to want to see pin numbers matching the manufacturer's data sheet, and manufacturers have no common numbering scheme. gEDA can't unilaterally fix these problems. Got it, and that answers my question pretty well. For a more complex project, I generally want some project-specific default attributes like footprint=0603 and spec=1/16W,5%. The customer, layout contractor, and application have an influence here. Now I understand why you make per-project libraries. Please bear with me, I'm just a hobbyist. I've never had to work with a contractor or manufacturer. -- Amand Tihon 13C Rue Arsène Matton, 1325 Dion-Valmont, Belgium +32 479 207 743 signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
I think it's far more important to have the symbol browser import symbols into the *project* (not the schematic) as they are selected, so they can be customized as necessary. And it should pop up an annoying information box reminding the user to check the symbol until the user turns the box off. John Doty Noqsi Aerospace, Ltd. If this means adding a footprint viewer and editor to the gschem application, and defining a default directory to store 'tweaked' footprints for that project (., or .gaf/packages, etc) then I would still consider that a HUGE improvement over what we have to work with now. I use gEDA on and off, so I do not get enough experience to quickly and efficiently find, make, modify footprints. Having to run a second window with pcb running does not help much, because what is easily visible to pcb may not be in the predefined directory structure of gschem, and therefore gsch2pcb. If there was a second library function/window/file browser in gschem, then if it could find the file, then I would be certain that gsch2pcb also would find it and it would cut way down on the 'element not found, pcb board is incomplete' runs I keep making. Or perhaps just a script or tools that will help set up all the resource files so that both programs access the same directories. I am new enough to Linux that it is not always obvious to me that a resource file is missing, has the wrong information, or the syntax is off and I never see a warning message that it is wrong, only that my board is once again incomplete. Mike ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Matching footprints with symbols
On Apr 14, 2010, at 3:46 PM, Mike Bushroe wrote: I think it's far more important to have the symbol browser import symbols into the *project* (not the schematic) as they are selected, so they can be customized as necessary. And it should pop up an annoying information box reminding the user to check the symbol until the user turns the box off. John Doty Noqsi Aerospace, Ltd. If this means adding a footprint viewer and editor to the gschem application, and defining a default directory to store 'tweaked' footprints for that project (., or .gaf/packages, etc) then I would still consider that a HUGE improvement over what we have to work with now. No, that's not what I'm talking about. Footprints depend on the layout tool: gschem is properly agnostic about what layout tool you're using. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
