kicad-developers team mailing list archive
-
kicad-developers team
-
Mailing list archive
-
Message #35985
Re: More default fields in schematic
We really must choose a model. What we have is broken under either model.
If they’re “default” fields, then they need to be there by default. That’s what “default” means. I understand this isn’t the model you have in mind.
The alternative is “seed” (or “template”) fields. In this model they must be added by the user. But that’s NOT what the code does (either before or after the recent change). If you edit a symbol they are *silently* added (as if they were default fields). If you understand the model to be seed fields, and all you did was change the symbol orientation, having the seed fields added will be VERY surprising.
This is why I suggested earlier that if we want to treat them as seed fields then we need a button in the Symbol Properties dialog to add the fields. That way it’s clear to everyone what is happening.
> On 29 May 2018, at 16:30, Wayne Stambaugh <stambaughw@xxxxxxxxx> wrote:
>
> I figured out what is going on here. There are two distinct issues at play.
>
> It appears that all of the python BOM generation scripts[1] are adding
> non-mandatory fields even if the fields do not exist in the the generic
> (XML) netlist file. These should be fixed. I have no idea how much
> work this will be but a quick scan would suggest that it wouldn't be too
> difficult. I suspect these were provided as examples to create your own
> scripts. Used as is, they will add extra empty field columns to the
> BOM. BOMs generated with xsltproc do not exhibit this issue so the as
> long as the default field does not have a value associated with it, the
> generic netlist file does not contain any unexpected field information.
>
> However, if a default field contains a value then it is added to the
> default netlist even if none of the symbols contain said field. This is
> where I take exception. The generic netlist file should only contain
> fields that are defined in the symbols. The assumption that the netlist
> should contain default fields if the are not empty is broken. This will
> lead to corrupted BOMs for existing projects which is not acceptable.
> This change needs to be reverted. I know that it was done to fix a bug
> report but this is not an acceptable solution for the bug. We can push
> that bug fix off until the first v5 point release or v6 because it will
> require a feature change to fix.
>
> [1]: https://git.launchpad.net/kicad/tree/eeschema/plugins/python_scripts
>
> On 5/29/2018 10:12 AM, Jeff Young wrote:
>> Hi Reece,
>>
>> Was that generated with a recent build? Earlier versions of 5.0
>> certainly had that bug, but I’m pretty sure it’s been fixed.
>>
>> Cheers,
>> Jeff.
>>
>>
>>> On 29 May 2018, at 13:54, Reece R. Pollack <reece@xxxxxxx
>>> <mailto:reece@xxxxxxx>> wrote:
>>>
>>> On 05/29/18 08:27, Jeff Young wrote:
>>>> Comments inline:
>>>>
>>>>> On 28 May 2018, at 17:28, Reece R. Pollack <reece@xxxxxxx
>>>>> <mailto:reece@xxxxxxx>> wrote:
>>>>>
>>>>> I believe you owe me 2c. We can discuss 2c in which currency later. :-)
>>>>>
>>>>> I have five custom default fields defined:
>>>>> - Mfgr
>>>>> - Mfgr P/N
>>>>> - Dist
>>>>> - Dist P/N
>>>>> - Specifications
>>>>
>>>> None of these have any default values that make any sense, so I
>>>> assume they’re all just names with empty values, right?
>>>
>>> Yes, all of these are empty by default, though I typically order from
>>> DigiKey so I could have set that one. I added them as "Default Fields"
>>> so that all components would have the same fields, and I wouldn't have
>>> to depend on adding the field names by hand.
>>>
>>>>
>>>>>
>>>>> The first two give the manufacturer's name and part number; the
>>>>> second two give the distributor's name and part number; the third is
>>>>> a catch-all for specs that are important for ordering but aren't
>>>>> worth cluttering the schematic with.
>>>>>
>>>>> My biggest issue with the current Default Fields is that I didn't
>>>>> start my current project with them, so using the field edit
>>>>> spreadsheet-like thingie often results in lots of noise in my
>>>>> commits as the empty default fields get added to components.
>>>>
>>>> If it’s adding empty default fields then it’s a bug. It should only
>>>> add them if they have non-empty values.
>>>
>>> Then you have a bug. Here's a small excerpt from a Git diff where a
>>> lot of components had empty fields added. None of these components
>>> were added in this revision; I was simply setting part numbers for
>>> /other/ components using the field editor spreadsheet thingie:
>>>
>>> diff --git a/Recreation/P170-DH/pcb/P170-DH
>>> Replacement/ExternalInterface.sch b/Recreation/P170-DH/pcb/P170-DH
>>> Replacement/ExternalInterface.sch
>>> index 37482ee..e2aea43 100644
>>> --- a/Recreation/P170-DH/pcb/P170-DH Replacement/ExternalInterface.sch
>>> +++ b/Recreation/P170-DH/pcb/P170-DH Replacement/ExternalInterface.sch
>>> @@ -22,6 +22,11 @@ F 0 "U12" H 3900 2215 50 0000 C CNN
>>> F 1 "74LVC1T45" H 3900 2124 50 0000 C CNN
>>> F 2 "Package_TO_SOT_SMD:SOT-23-6" H 3900 1850 50 0001 C CNN
>>> F 3 "http://www.ti.com/lit/ds/symlink/sn74lvc1t45.pdf"; H 3900 1850
>>> 50 0001 C CNN
>>> +F 4 "" H 0 0 50 0001 C CNN "Distr"
>>> +F 5 "" H 0 0 50 0001 C CNN "Distr P/N"
>>> +F 6 "" H 0 0 50 0001 C CNN "Mfgr"
>>> +F 7 "" H 0 0 50 0001 C CNN "Mfgr P/N"
>>> +F 8 "" H 0 0 50 0001 C CNN "Specifications"
>>> 1 3900 1850
>>> 1 0 0 -1
>>> $EndComp
>>> @@ -33,6 +38,11 @@ F 0 "U13" H 3900 3415 50 0000 C CNN
>>> F 1 "74LVC1T45" H 3900 3324 50 0000 C CNN
>>> F 2 "Package_TO_SOT_SMD:SOT-23-6" H 3900 3050 50 0001 C CNN
>>> F 3 "http://www.ti.com/lit/ds/symlink/sn74lvc1t45.pdf"; H 3900 3050
>>> 50 0001 C CNN
>>> +F 4 "" H 0 0 50 0001 C CNN "Distr"
>>> +F 5 "" H 0 0 50 0001 C CNN "Distr P/N"
>>> +F 6 "" H 0 0 50 0001 C CNN "Mfgr"
>>> +F 7 "" H 0 0 50 0001 C CNN "Mfgr P/N"
>>> +F 8 "" H 0 0 50 0001 C CNN "Specifications"
>>> 1 3900 3050
>>> 1 0 0 -1
>>> $EndComp
>>> @@ -66,6 +86,11 @@ F 0 "J5" H 7719 1375 50 0000 C CNN
>>> F 1 "Conn_01x06" H 7719 1466 50 0000 C CNN
>>> F 2 "Connector_PinHeader_2.54mm:PinHeader_1x06_P2.54mm_Vertical" H
>>> 7800 1900 50 0001 C CNN
>>> F 3 "~" H 7800 1900 50 0001 C CNN
>>> +F 4 "" H 0 0 50 0001 C CNN "Distr"
>>> +F 5 "" H 0 0 50 0001 C CNN "Distr P/N"
>>> +F 6 "" H 0 0 50 0001 C CNN "Mfgr"
>>> +F 7 "" H 0 0 50 0001 C CNN "Mfgr P/N"
>>> +F 8 "" H 0 0 50 0001 C CNN "Specifications"
>>> 1 7800 1900
>>> 1 0 0 -1
>>> $EndComp
>>> @@ -209,6 +234,7 @@ F 4 "CTS" H 3900 7100 50 0001 C CNN "Mfgr"
>>> F 5 "218-4LPST" H 3900 7100 50 0001 C CNN "Mfgr P/N"
>>> F 6 "DigiKey" H 3900 7100 50 0001 C CNN "Distr"
>>> F 7 "CT2184LPST-ND" H 3900 7100 50 0001 C CNN "Distr P/N"
>>> +F 8 "" H 0 0 50 0001 C CNN "Specifications"
>>> 1 3900 7100
>>> 1 0 0 -1
>>> $EndComp
>>> @@ -321,6 +347,11 @@ F 0 "R127" H 4509 5746 50 0000 L CNN
>>> F 1 "100K" H 4509 5655 50 0000 L CNN
>>> F 2 "Resistor_SMD:R_0603_1608Metric" H 4450 5700 50 0001 C CNN
>>> F 3 "~" H 4450 5700 50 0001 C CNN
>>> +F 4 "" H 0 0 50 0001 C CNN "Distr"
>>> +F 5 "" H 0 0 50 0001 C CNN "Distr P/N"
>>> +F 6 "" H 0 0 50 0001 C CNN "Mfgr"
>>> +F 7 "" H 0 0 50 0001 C CNN "Mfgr P/N"
>>> +F 8 "" H 0 0 50 0001 C CNN "Specifications"
>>> 1 4450 5700
>>> 1 0 0 -1
>>> $EndComp
>>>
>>>
>>>
>>>
>>>>
>>>> Cheers,
>>>> Jeff.
>>>>
>>>>>
>>>>> I was originally against adding such defined fields, as I expect it
>>>>> will add fields to components that will potentially conflict with
>>>>> those created by current users. However, if it doesn't do that, and
>>>>> has the support from parts distributors, I guess I could live with it.
>>>>>
>>>>> On 05/22/18 10:56, Fabrizio Tappero wrote:
>>>>>> Hello,
>>>>>> I'd like to contribute with my 2c.
>>>>>>
>>>>>> I completely agree with Kristoffer, there is a need for a "MPN"
>>>>>> field hard coded exactly as "Value" field is hard coded in Kicad.
>>>>>>
>>>>>> As Wayne mentions the current "Preferences - General Options -
>>>>>> Default Fields" is not a bad option to add a "MPN" field. This is
>>>>>> what I do and this is what all my PCB colleges at work do.
>>>>>>
>>>>>> Above solution will however not help the majority to do the same. I
>>>>>> would actually bet 2c that nearly nobody uses the Default Fields
>>>>>> feature (most of the people probably do it component by component).
>>>>>> And this makes it a not so useful feature.
>>>>>>
>>>>>> Kicost is a god-made tool and for sure Dave will soon add MPN as a
>>>>>> default field in Kicad.
>>>>>>
>>>>>> Cheers
>>>>>> Fabrizio
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>> On Tue, May 22, 2018 at 3:41 PM, kristoffer ödmark
>>>>>> <kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>> wrote:
>>>>>>
>>>>>> My updated patch forgot to add the files before doing the --amend.
>>>>>>
>>>>>> So it only updated the commit message. Here is the real file
>>>>>>
>>>>>> On Tue, 2018-05-22 at 07:52 -0500, Ben Hest wrote:
>>>>>>> From a Digi-Key KiCad library standpoint, as we're still in
>>>>>> beta, I
>>>>>>> would
>>>>>>> gladly change the fields to whatever would be decided.
>>>>>> Uniformity
>>>>>>> for
>>>>>>> plugins use would definitely be an advantage.
>>>>>>>
>>>>>>> -Ben
>>>>>>>
>>>>>>> On Tue, May 22, 2018 at 5:38 AM kristoffer ödmark <
>>>>>>> kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>> wrote:
>>>>>>>
>>>>>>>> Thanks! This is exactly what i was going for, non-intrusive
>>>>>>>> oppurtunity
>>>>>>>> for uniformity!
>>>>>>>>
>>>>>>>> I tested the bom2csv plugin, It did not include the empty
>>>>>> fields.
>>>>>>>>
>>>>>>>> I also tested the bom_csv_sorted_by_ref, it did not include the
>>>>>>>> empty
>>>>>>>> values, but it included some values I had not specified,
>>>>>> such as
>>>>>>>> Manufacturer and Vendor even if they were not provided in the
>>>>>>>> schematic.
>>>>>>>>
>>>>>>>> - Kristoffer
>>>>>>>>
>>>>>>>> On Tue, 2018-05-22 at 11:05 +0100, Jeff Young wrote:
>>>>>>>>> I think I like this new patch. It provides the
>>>>>> /opportunity/ for
>>>>>>>>> uniformity, without getting in the way of those who want
>>>>>> to go
>>>>>>>>> their
>>>>>>>>> own way.
>>>>>>>>>
>>>>>>>>> Do the BOM generators automatically output all default
>>>>>> fields or
>>>>>>>>> only
>>>>>>>>> those with values?
>>>>>>>>>
>>>>>>>>>> On 22 May 2018, at 09:22, kristoffer ödmark
>>>>>> <kristofferodmark90
>>>>>>>>>> @gma
>>>>>>>>>> il.com <http://il.com/>> wrote:
>>>>>>>>>>
>>>>>>>>>> Please disregard my previous mail, it got mangled badly
>>>>>>>>>> somehow, it
>>>>>>>>>> did
>>>>>>>>>> not look like that in my editor at least.
>>>>>>>>>>
>>>>>>>>>> On Mon, 2018-05-21 at 18:22 -0400, Wayne Stambaugh wrote:
>>>>>>>>>>> Eeschema already supports creating default optional
>>>>>> fields in
>>>>>>>>>>> the
>>>>>>>>>>> configuration settings dialog. Used correctly, these
>>>>>> will
>>>>>>>>>>> give
>>>>>>>>>>> you
>>>>>>>>>>> the
>>>>>>>>>>> same optional field names for every project without
>>>>>> having to
>>>>>>>>>>> add
>>>>>>>>>>> them
>>>>>>>>>>> by hand to each symbol and possibly typing in
>>>>>> different field
>>>>>>>>>>> names
>>>>>>>>>>> by
>>>>>>>>>>> accident.
>>>>>>>>>>
>>>>>>>>>> Different users will still type in different field
>>>>>> names for
>>>>>>>>>> the
>>>>>>>>>> same
>>>>>>>>>> things though. What you describe works as long as there
>>>>>> is only
>>>>>>>>>> one
>>>>>>>>>> person in the entire projects lifetime, using only one
>>>>>>>>>> computer.
>>>>>>>>>>
>>>>>>>>>>> The proposed patch would intermingle the default fields
>>>>>>>>>>> with
>>>>>>>>>>> existing schematic symbol fields which would break
>>>>>> existing
>>>>>>>>>>> BOMs
>>>>>>>>>>> which I
>>>>>>>>>>> don't think users will appreciate.
>>>>>>>>>>
>>>>>>>>>> The proposed patch will only change default settings,
>>>>>> existing
>>>>>>>>>> users
>>>>>>>>>> with a config already in place will not be affected. I
>>>>>> realised
>>>>>>>>>> that
>>>>>>>>>> the fields now accept empty values as well, so existing
>>>>>> boms on
>>>>>>>>>> new
>>>>>>>>>> installations will not be affected either. I updated
>>>>>> the patch,
>>>>>>>>>> so
>>>>>>>>>> it
>>>>>>>>>> will not affect anyone that doesnt use the fields.
>>>>>>>>>>
>>>>>>>>>>> [...] As I've stated before, I can set 10
>>>>>>>>>>> different designers down and I will get 10 different
>>>>>> sets of
>>>>>>>>>>> default
>>>>>>>>>>> field names. This really seems like me to be a
>>>>>> configuration
>>>>>>>>>>> issue.
>>>>>>>>>>
>>>>>>>>>> This is the problems I want to address, because those 10
>>>>>>>>>> designers
>>>>>>>>>> will
>>>>>>>>>> by experience also spell the same field in 10 different
>>>>>> ways.
>>>>>>>>>> Making
>>>>>>>>>> their fields incompatable. MPN, MFPN, #mfg, ManufPart,
>>>>>> etc etc.
>>>>>>>>>> Let
>>>>>>>>>> those 10 designers remove the fields they do not want
>>>>>> instead.
>>>>>>>>>>
>>>>>>>>>>> The only possible solution that I would accept is to
>>>>>> move the
>>>>>>>>>>> default
>>>>>>>>>>> field definitions from the eeschema configuration
>>>>>> file into
>>>>>>>>>>> the
>>>>>>>>>>> default
>>>>>>>>>>> kicad project file. This way existing projects would
>>>>>> not be
>>>>>>>>>>> polluted
>>>>>>>>>>> with the proposed default fields and users could
>>>>>> define their
>>>>>>>>>>> own
>>>>>>>>>>> default fields in a custom project file.
>>>>>>>>>>
>>>>>>>>>> Default fields does not pollute if they are empty, they
>>>>>> just
>>>>>>>>>> give a
>>>>>>>>>> hint of what data could be put into the schematic, same
>>>>>> as with
>>>>>>>>>> the
>>>>>>>>>> datasheet field, which is not often used. Funny how
>>>>>> noone ever
>>>>>>>>>> complains about that one.
>>>>>>>>>>
>>>>>>>>>>> [...]
>>>>>>>>>>> A more flexible solution would be to add a "File->New
>>>>>> from
>>>>>>>>>>> Custom
>>>>>>>>>>> Template" command to KiCad to allow the user to
>>>>>> select any
>>>>>>>>>>> custom
>>>>>>>>>>> project file. This would allow for multiple custom
>>>>>> project
>>>>>>>>>>> files
>>>>>>>>>>> instead of forcing the user to use only a single default
>>>>>>>>>>> project
>>>>>>>>>>> file.
>>>>>>>>>>
>>>>>>>>>> As long as the "File->New Project" would include the
>>>>>> additional
>>>>>>>>>> fields
>>>>>>>>>> and then people can use "New from Custom Template"
>>>>>> means they
>>>>>>>>>> can
>>>>>>>>>> use a
>>>>>>>>>> template that is empty. Otherwise it would defeat the
>>>>>> purpose.
>>>>>>>>>> I am
>>>>>>>>>> proposing a slightly different default configuration,
>>>>>> not any
>>>>>>>>>> change in
>>>>>>>>>> how people will use the software.
>>>>>>>>>>
>>>>>>>>>>> Cheers,
>>>>>>>>>>>
>>>>>>>>>>> Wayne
>>>>>>>>>>>
>>>>>>>>>>> On 05/20/2018 06:27 PM, Andrey Kuznetsov wrote:
>>>>>>>>>>>> I agree, I had the same issue when I was doing my
>>>>>> board, I
>>>>>>>>>>>> needed a
>>>>>>>>>>>> field for all components, and I had to manually add
>>>>>> it for
>>>>>>>>>>>> every
>>>>>>>>>>>> item,
>>>>>>>>>>>> there was no way to add this field to all
>>>>>> components at the
>>>>>>>>>>>> same
>>>>>>>>>>>> time or
>>>>>>>>>>>> to have it add by default from the addition of a new
>>>>>>>>>>>> component
>>>>>>>>>>>> to
>>>>>>>>>>>> the sheet.
>>>>>>>>>>>>
>>>>>>>>>>>> Which reminds me, Cadence Designer has tools to
>>>>>> manipulate
>>>>>>>>>>>> fields
>>>>>>>>>>>> on a
>>>>>>>>>>>> large scale, whether to add, delete, show, hide,
>>>>>> etc, this
>>>>>>>>>>>> is
>>>>>>>>>>>> something
>>>>>>>>>>>> that would be nice to have in KiCAD, either that or
>>>>>> a table
>>>>>>>>>>>> of
>>>>>>>>>>>> all
>>>>>>>>>>>> components for the sheet or schematic and columns
>>>>>> for each
>>>>>>>>>>>> field,
>>>>>>>>>>>> with
>>>>>>>>>>>> ability to show/hide each cell individually.
>>>>>>>>>>>>
>>>>>>>>>>>> I think the ultimate goal is to make the Symbol
>>>>>> Table more
>>>>>>>>>>>> useful,
>>>>>>>>>>>> but
>>>>>>>>>>>> that'll take to long for v5 so if Kristoffer's
>>>>>> patch allows
>>>>>>>>>>>> an
>>>>>>>>>>>> easy
>>>>>>>>>>>> way
>>>>>>>>>>>> to add fields to all components or similar, I'd say
>>>>>> do it
>>>>>>>>>>>> because
>>>>>>>>>>>> people
>>>>>>>>>>>> will be pissed and waste their time doing it for every
>>>>>>>>>>>> component in
>>>>>>>>>>>> their schematic.
>>>>>>>>>>>>
>>>>>>>>>>>> On Sun, May 20, 2018 at 3:01 PM, kristoffer Ödmark
>>>>>>>>>>>> <kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>
>>>>>> <mailto:kristofferodmark90@gm <mailto:kristofferodmark90@gm>
>>>>>>>>>>>> ail.
>>>>>>>>>>>> com>
>>>>>>>>>>>>> wrote:
>>>>>>>>>>>>
>>>>>>>>>>>> I obvviously disagree, the correct solution
>>>>>> would be to
>>>>>>>>>>>> have
>>>>>>>>>>>> both.
>>>>>>>>>>>> This does not hinder that, its not even the same
>>>>>>>>>>>> problem.
>>>>>>>>>>>>
>>>>>>>>>>>> The problem is for everyone who want for example the
>>>>>>>>>>>> Manufacturer
>>>>>>>>>>>> Part Number will have to define a fieldname,
>>>>>> which every
>>>>>>>>>>>> time
>>>>>>>>>>>> results in them abbreviating it to something
>>>>>> different.
>>>>>>>>>>>> Hence
>>>>>>>>>>>> nobody
>>>>>>>>>>>> can work with Manufacturer Part Numbers.
>>>>>>>>>>>>
>>>>>>>>>>>> Here is something similar, Imagine all of the
>>>>>> colours in
>>>>>>>>>>>> Kicad
>>>>>>>>>>>> for
>>>>>>>>>>>> all of the layers where white by default. Have fun
>>>>>>>>>>>> defining
>>>>>>>>>>>> all
>>>>>>>>>>>> the
>>>>>>>>>>>> colours yourself.
>>>>>>>>>>>> Maybe you want to define them yourself, nobody is
>>>>>>>>>>>> stopping
>>>>>>>>>>>> you
>>>>>>>>>>>> now
>>>>>>>>>>>> either, just get cracking.
>>>>>>>>>>>>
>>>>>>>>>>>> How easy would it be for you to look at the board
>>>>>>>>>>>> someone
>>>>>>>>>>>> else
>>>>>>>>>>>> made
>>>>>>>>>>>> later and understand what is what? Maybe for
>>>>>> some that
>>>>>>>>>>>> is a
>>>>>>>>>>>> better
>>>>>>>>>>>> solution, but for me that
>>>>>>>>>>>> would be an extreme example of bad default values.
>>>>>>>>>>>>
>>>>>>>>>>>> This is how the default fields are now, they are
>>>>>> white,
>>>>>>>>>>>> or
>>>>>>>>>>>> more
>>>>>>>>>>>> like
>>>>>>>>>>>> see-throught, which makes life harder for anyone
>>>>>> that
>>>>>>>>>>>> wants to contribute or create tools that
>>>>>> interact with
>>>>>>>>>>>> kicad,
>>>>>>>>>>>> and as
>>>>>>>>>>>> I previously said, this is only a default, you
>>>>>> are still
>>>>>>>>>>>> equally able to add/remove or change the fields
>>>>>> how you
>>>>>>>>>>>> want
>>>>>>>>>>>> to.
>>>>>>>>>>>> But, tools like kibom or various other web-based
>>>>>> tools
>>>>>>>>>>>> can
>>>>>>>>>>>> much
>>>>>>>>>>>> easier integrate to it, or at least support a
>>>>>> default
>>>>>>>>>>>> value
>>>>>>>>>>>> as
>>>>>>>>>>>> well.
>>>>>>>>>>>> So for the majority of users, who doesnt change
>>>>>>>>>>>> defaults,
>>>>>>>>>>>> the tool would just work.
>>>>>>>>>>>>
>>>>>>>>>>>> I will reiterate, I do not care what they are
>>>>>> named, I
>>>>>>>>>>>> want
>>>>>>>>>>>> a
>>>>>>>>>>>> default field where I can put my manufacturer part
>>>>>>>>>>>> number,
>>>>>>>>>>>> amongs
>>>>>>>>>>>> others.
>>>>>>>>>>>> The specific abbreviation or name does not
>>>>>> matter, If i
>>>>>>>>>>>> care, I
>>>>>>>>>>>> can
>>>>>>>>>>>> manually add/remove my own fields *JUST AS I DO
>>>>>> NOW*,
>>>>>>>>>>>> but
>>>>>>>>>>>> for
>>>>>>>>>>>> the people
>>>>>>>>>>>> who use it, it will be easier across projects,
>>>>>> for the
>>>>>>>>>>>> people
>>>>>>>>>>>> that
>>>>>>>>>>>> dont, It will not matter.
>>>>>>>>>>>>
>>>>>>>>>>>> Sane defaults matter. A lot actually.
>>>>>>>>>>>>
>>>>>>>>>>>> - Kristoffer
>>>>>>>>>>>>
>>>>>>>>>>>> On 2018-05-20 23:40, José Ignacio wrote:
>>>>>>>>>>>>
>>>>>>>>>>>> I dont like this, the right solution would be to
>>>>>>>>>>>> allow
>>>>>>>>>>>> for
>>>>>>>>>>>> importing a default config into kicad for things
>>>>>>>>>>>> like
>>>>>>>>>>>> that,
>>>>>>>>>>>> as
>>>>>>>>>>>> different groups will have different policies.
>>>>>>>>>>>>
>>>>>>>>>>>> On Sun, May 20, 2018 at 3:31 PM, Kristoffer
>>>>>> Ödmark
>>>>>>>>>>>> <kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>>>> wrote:
>>>>>>>>>>>>
>>>>>>>>>>>> The patch should only affect first startup,
>>>>>>>>>>>> changes
>>>>>>>>>>>> to
>>>>>>>>>>>> the
>>>>>>>>>>>> fields
>>>>>>>>>>>> will be saved
>>>>>>>>>>>>
>>>>>>>>>>>> On May 20, 2018 22:18, "Seth Hillbrand"
>>>>>>>>>>>> <seth.hillbrand@xxxxxxxxx
>>>>>> <mailto:seth.hillbrand@xxxxxxxxx> <mailto:seth.hillbrand@gma
>>>>>> <mailto:seth.hillbrand@gma>
>>>>>>>>>>>> il.c
>>>>>>>>>>>> om>
>>>>>>>>>>>> <mailto:seth.hillbrand@xxxxxxxxx
>>>>>> <mailto:seth.hillbrand@xxxxxxxxx>
>>>>>>>>>>>> <mailto:seth.hillbrand@xxxxxxxxx
>>>>>> <mailto:seth.hillbrand@xxxxxxxxx>>>> wrote:
>>>>>>>>>>>>
>>>>>>>>>>>> Hi Kristoffer-
>>>>>>>>>>>>
>>>>>>>>>>>> This feels like a management issue
>>>>>> rather
>>>>>>>>>>>> than a
>>>>>>>>>>>> tool
>>>>>>>>>>>> issue.
>>>>>>>>>>>> If the user doesn't want any extra
>>>>>> fields,
>>>>>>>>>>>> how
>>>>>>>>>>>> would your
>>>>>>>>>>>> patch allow that?
>>>>>>>>>>>>
>>>>>>>>>>>> -S
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> Am So., 20. Mai 2018 um 13:00 Uhr
>>>>>> schrieb
>>>>>>>>>>>> kristoffer Ödmark
>>>>>>>>>>>> <kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>
>>>>>>>>>>>> <mailto:kristofferodmark90@xxxxxxxxx
>>>>>> <mailto:kristofferodmark90@xxxxxxxxx>>>>:
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> Hello!
>>>>>>>>>>>>
>>>>>>>>>>>> I will open this can of worms
>>>>>> again, I
>>>>>>>>>>>> feel
>>>>>>>>>>>> that I have
>>>>>>>>>>>> to. So from what
>>>>>>>>>>>> I gather we have proffessionals
>>>>>> as the
>>>>>>>>>>>> main
>>>>>>>>>>>> aim
>>>>>>>>>>>> in
>>>>>>>>>>>> Kicad.
>>>>>>>>>>>> The reason I will open this
>>>>>> issue again
>>>>>>>>>>>> is
>>>>>>>>>>>> that
>>>>>>>>>>>> I
>>>>>>>>>>>> feel we
>>>>>>>>>>>> have a
>>>>>>>>>>>> collaboration issue, maybe not a
>>>>>> mayor
>>>>>>>>>>>> one.
>>>>>>>>>>>> But
>>>>>>>>>>>> one
>>>>>>>>>>>> nonetheless.
>>>>>>>>>>>>
>>>>>>>>>>>> We really need more default
>>>>>> fields for
>>>>>>>>>>>> our
>>>>>>>>>>>> schematic
>>>>>>>>>>>> symbols. Im not
>>>>>>>>>>>> proposing required fields, I am
>>>>>> *ONLY*
>>>>>>>>>>>> proposing that
>>>>>>>>>>>> there should be default fields added
>>>>>>>>>>>> into
>>>>>>>>>>>> the
>>>>>>>>>>>> default
>>>>>>>>>>>> fields settings
>>>>>>>>>>>> tab. I am not proposing they
>>>>>> need to be
>>>>>>>>>>>> filled
>>>>>>>>>>>> in the
>>>>>>>>>>>> libraries, nor that people need
>>>>>> to use
>>>>>>>>>>>> them.
>>>>>>>>>>>> only that
>>>>>>>>>>>> they need to
>>>>>>>>>>>> exist with a fresh install of
>>>>>> kicad so
>>>>>>>>>>>> that
>>>>>>>>>>>> easy
>>>>>>>>>>>> problems
>>>>>>>>>>>> such as theese do not happen:
>>>>>>>>>>>>
>>>>>>>>>>>> - Collaborators working on
>>>>>> the same
>>>>>>>>>>>> project
>>>>>>>>>>>> will not
>>>>>>>>>>>> create
>>>>>>>>>>>> duplicate fields in libs/projects
>>>>>>>>>>>> describing
>>>>>>>>>>>> the same
>>>>>>>>>>>> thing by mistake
>>>>>>>>>>>> - Projects that aim to
>>>>>> interact or
>>>>>>>>>>>> add
>>>>>>>>>>>> to
>>>>>>>>>>>> Kicad can
>>>>>>>>>>>> assume that the
>>>>>>>>>>>> Fields will exist, and will know
>>>>>> what
>>>>>>>>>>>> name/tag
>>>>>>>>>>>> to
>>>>>>>>>>>> look for
>>>>>>>>>>>> (bom exporters, price
>>>>>> checkers,
>>>>>>>>>>>> MacroFab, etc)
>>>>>>>>>>>> - Open source projects will be
>>>>>>>>>>>> easier
>>>>>>>>>>>> to
>>>>>>>>>>>> collaborate,
>>>>>>>>>>>> read and order
>>>>>>>>>>>>
>>>>>>>>>>>> The reason I think it is better
>>>>>> to have
>>>>>>>>>>>> the
>>>>>>>>>>>> fields by
>>>>>>>>>>>> default than the
>>>>>>>>>>>> current solution to add them is
>>>>>> that the
>>>>>>>>>>>> majority
>>>>>>>>>>>> will use
>>>>>>>>>>>> what exists, and tools can
>>>>>> support it
>>>>>>>>>>>> from
>>>>>>>>>>>> the
>>>>>>>>>>>> very
>>>>>>>>>>>> beginning, people
>>>>>>>>>>>> with inhouse tools seems to dislike
>>>>>>>>>>>> this,
>>>>>>>>>>>> since
>>>>>>>>>>>> they
>>>>>>>>>>>> map their
>>>>>>>>>>>> parts with an inhouse number -
>>>>>> and then
>>>>>>>>>>>> handle
>>>>>>>>>>>> the
>>>>>>>>>>>> information about the
>>>>>>>>>>>> part there. From what I gather,
>>>>>> this is
>>>>>>>>>>>> not
>>>>>>>>>>>> the
>>>>>>>>>>>> majority, and
>>>>>>>>>>>> these persons still modify the
>>>>>> default
>>>>>>>>>>>> fields
>>>>>>>>>>>> settings.
>>>>>>>>>>>>
>>>>>>>>>>>> I spent maybe 30-40 mins
>>>>>> checking the
>>>>>>>>>>>> "made
>>>>>>>>>>>> with kicad"
>>>>>>>>>>>> projects, I
>>>>>>>>>>>> found that the most common
>>>>>> addition to
>>>>>>>>>>>> libs
>>>>>>>>>>>> and
>>>>>>>>>>>> schematics
>>>>>>>>>>>> are:
>>>>>>>>>>>> - Manufacturers part
>>>>>> number, these
>>>>>>>>>>>> were
>>>>>>>>>>>> named
>>>>>>>>>>>> widely
>>>>>>>>>>>> different in
>>>>>>>>>>>> projects, (BOM, MP, MPN, #mfg, or
>>>>>>>>>>>> different
>>>>>>>>>>>> syntaxes in
>>>>>>>>>>>> the Value field )
>>>>>>>>>>>> I even saw a mix of
>>>>>> these in
>>>>>>>>>>>> the
>>>>>>>>>>>> same
>>>>>>>>>>>> project
>>>>>>>>>>>> once, along with
>>>>>>>>>>>> some people having the vendor id
>>>>>> only.
>>>>>>>>>>>> - Manufacturer ( found some
>>>>>>>>>>>> different
>>>>>>>>>>>> languages
>>>>>>>>>>>> though )
>>>>>>>>>>>>
>>>>>>>>>>>> more uncommon things was, Tolerance(
>>>>>>>>>>>> 10%,
>>>>>>>>>>>> 20pps),
>>>>>>>>>>>> Ratings
>>>>>>>>>>>> ( 1/4W, 85C,
>>>>>>>>>>>> 16V ), Vendor information and
>>>>>> different
>>>>>>>>>>>> Descriptions. They
>>>>>>>>>>>> were named
>>>>>>>>>>>> and abbreviated
>>>>>>>>>>>> very differently accross projects.
>>>>>>>>>>>>
>>>>>>>>>>>> What I would like to see is these
>>>>>>>>>>>> additional
>>>>>>>>>>>> fields by
>>>>>>>>>>>> default, but
>>>>>>>>>>>> hidden from the schematic unless
>>>>>> changed
>>>>>>>>>>>> by
>>>>>>>>>>>> user.
>>>>>>>>>>>> Tolerance ( used for setting
>>>>>>>>>>>> tolerances
>>>>>>>>>>>> of
>>>>>>>>>>>> resistors,
>>>>>>>>>>>> capacitors,
>>>>>>>>>>>> oscillators, etc )
>>>>>>>>>>>> MaxRating ( field were one can
>>>>>>>>>>>> specify
>>>>>>>>>>>> max
>>>>>>>>>>>> Voltage,
>>>>>>>>>>>> Ampere,
>>>>>>>>>>>> Frequency, or whatever the component
>>>>>>>>>>>> needs )
>>>>>>>>>>>> Manufacturer ( For inhouse
>>>>>> numbers,
>>>>>>>>>>>> they
>>>>>>>>>>>> could
>>>>>>>>>>>> either
>>>>>>>>>>>> just remove
>>>>>>>>>>>> it, or use the company/group name )
>>>>>>>>>>>> MPN ( Maybe PartNumber could be
>>>>>>>>>>>> used
>>>>>>>>>>>> here,
>>>>>>>>>>>> and
>>>>>>>>>>>> people
>>>>>>>>>>>> who use
>>>>>>>>>>>> inhouse numbers use it aswell, I
>>>>>> dont
>>>>>>>>>>>> really
>>>>>>>>>>>> care
>>>>>>>>>>>> what its
>>>>>>>>>>>> called, as
>>>>>>>>>>>> long as its called something )
>>>>>>>>>>>> Vendor
>>>>>>>>>>>> Notes
>>>>>>>>>>>>
>>>>>>>>>>>> I would be all up for extra
>>>>>>>>>>>> additions/removals,
>>>>>>>>>>>> but I
>>>>>>>>>>>> would prefer if
>>>>>>>>>>>> the naming is not discussed, but
>>>>>> rather
>>>>>>>>>>>> just
>>>>>>>>>>>> decided/agreed upon by
>>>>>>>>>>>> someone in the lead team.
>>>>>>>>>>>> The very least I think should be
>>>>>> added
>>>>>>>>>>>> in
>>>>>>>>>>>> case
>>>>>>>>>>>> the
>>>>>>>>>>>> previous is to much are:
>>>>>>>>>>>> Tolerance
>>>>>>>>>>>> Manufacturer
>>>>>>>>>>>> MPN
>>>>>>>>>>>>
>>>>>>>>>>>> I attach a patch for the minimal
>>>>>> set,
>>>>>>>>>>>> tested
>>>>>>>>>>>> on
>>>>>>>>>>>> linux by
>>>>>>>>>>>> removing the
>>>>>>>>>>>> .config/kicad/eeschema file.
>>>>>>>>>>>>
>>>>>>>>>>>> - Kristoffer
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> ps
>>>>>>>>>>>> Some github files i reviewed,
>>>>>> not all:
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> https://github.com/AnaviTechnology/anavi-gardening/b
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/b>
>>>>>>>>>>>> lob/
>>>>>>>>>>>> mas
>>>>>>>>>>>> ter/MCP3002-I_SN.lib
>>>>>>>>>>>>
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/>
>>>>>>>>>>>> blob
>>>>>>>>>>>> /ma
>>>>>>>>>>>> ster/MCP3002-I_SN.lib>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/>
>>>>>>>>>>>> blob
>>>>>>>>>>>> /ma
>>>>>>>>>>>> ster/MCP3002-I_SN.lib
>>>>>>>>>>>>
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/
>>>>>> <https://github.com/AnaviTechnology/anavi-gardening/>
>>>>>>>>>>>> blob
>>>>>>>>>>>> /ma
>>>>>>>>>>>> ster/MCP3002-I_SN.lib>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> https://github.com/jonpe960/blixten/blob/master/Blix
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Blix>
>>>>>>>>>>>> ten%
>>>>>>>>>>>> 20L
>>>>>>>>>>>> ED%20Device/Blixten.sch
>>>>>>>>>>>>
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli>
>>>>>>>>>>>> xten
>>>>>>>>>>>> %20
>>>>>>>>>>>> LED%20Device/Blixten.sch>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli>
>>>>>>>>>>>> xten
>>>>>>>>>>>> %20
>>>>>>>>>>>> LED%20Device/Blixten.sch
>>>>>>>>>>>>
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli
>>>>>> <https://github.com/jonpe960/blixten/blob/master/Bli>
>>>>>>>>>>>> xten
>>>>>>>>>>>> %20
>>>>>>>>>>>> LED%20Device/Blixten.sch>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> https://github.com/paltatech/half-bridge/blob/master
>>>>>> <https://github.com/paltatech/half-bridge/blob/master>
>>>>>>>>>>>> /pcb
>>>>>>>>>>>> %20
>>>>>>>>>>>> design/IGBT_board-cache.lib
>>>>>>>>>>>>
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste>
>>>>>>>>>>>> r/pc
>>>>>>>>>>>> b%2
>>>>>>>>>>>> 0design/IGBT_board-cache.lib>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste>
>>>>>>>>>>>> r/pc
>>>>>>>>>>>> b%2
>>>>>>>>>>>> 0design/IGBT_board-cache.lib
>>>>>>>>>>>>
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste
>>>>>> <https://github.com/paltatech/half-bridge/blob/maste>
>>>>>>>>>>>> r/pc
>>>>>>>>>>>> b%2
>>>>>>>>>>>> 0design/IGBT_board-cache.lib>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> https://github.com/pluggee/KiCADLibs/blob/master/sch
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sch>
>>>>>>>>>>>> /cap
>>>>>>>>>>>> _sm
>>>>>>>>>>>> d.lib
>>>>>>>>>>>>
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc>
>>>>>>>>>>>> h/ca
>>>>>>>>>>>> p_s
>>>>>>>>>>>> md.lib>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc>
>>>>>>>>>>>> h/ca
>>>>>>>>>>>> p_s
>>>>>>>>>>>> md.lib
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc
>>>>>> <https://github.com/pluggee/KiCADLibs/blob/master/sc>
>>>>>>>>>>>> h/ca
>>>>>>>>>>>> p_sm
>>>>>>>>>>>> d.lib>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> https://github.com/jim17/memtype/blob/master/schemat
>>>>>> <https://github.com/jim17/memtype/blob/master/schemat>
>>>>>>>>>>>> ic_p
>>>>>>>>>>>> cb/
>>>>>>>>>>>> electronic_design_kicad/electronic_design_kicad.sch
>>>>>>>>>>>>
>>>>>> <https://github.com/jim17/memtype/blob/master/schema
>>>>>> <https://github.com/jim17/memtype/blob/master/schema>
>>>>>>>>>>>> tic_
>>>>>>>>>>>> pcb
>>>>>>>>>>>> /electronic_design_kicad/electronic_design_kicad.sch>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> <https://github.com/jim17/memtype/blob/master/schema
>>>>>> <https://github.com/jim17/memtype/blob/master/schema>
>>>>>>>>>>>> tic_
>>>>>>>>>>>> pcb
>>>>>>>>>>>> /electronic_design_kicad/electronic_design_kicad.sch
>>>>>>>>>>>>
>>>>>> <https://github.com/jim17/memtype/blob/master/schema
>>>>>> <https://github.com/jim17/memtype/blob/master/schema>
>>>>>>>>>>>> tic_
>>>>>>>>>>>> pcb
>>>>>>>>>>>> /electronic_design_kicad/electronic_design_kicad.sch>>
>>>>>>>>>>>>
>>>>>> ________________________________________
>>>>>>>>>>>> ____
>>>>>>>>>>>> ___
>>>>>>>>>>>> Mailing list:
>>>>>>>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>>
>>>>>> <https://launchpad.net/%7Ekicad-develope
>>>>>> <https://launchpad.net/%7Ekicad-develope>
>>>>>>>>>>>> rs
>>>>>>>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>>
>>>>>>>>>>>> Post to :
>>>>>> kicad-developers@xxxxxxxxx
>>>>>>>>>>>> nchp
>>>>>>>>>>>> ad.
>>>>>>>>>>>> net
>>>>>>>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>>
>>>>>>>>>>>>
>>>>>> <mailto:kicad-developers@lists.launchpad
>>>>>> <mailto:kicad-developers@lists.launchpad>
>>>>>>>>>>>> .net
>>>>>>>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>>>
>>>>>>>>>>>> Unsubscribe :
>>>>>>>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>>
>>>>>> <https://launchpad.net/%7Ekicad-develope
>>>>>> <https://launchpad.net/%7Ekicad-develope>
>>>>>>>>>>>> rs
>>>>>>>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>>
>>>>>>>>>>>> More help :
>>>>>> https://help.launchpad.net <https://help.launchpad.net/>
>>>>>>>>>>>> /Lis
>>>>>>>>>>>> tHe
>>>>>>>>>>>> lp
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>>
>>>>>>>>>>>>
>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>> _______________________________________________
>>>>>>>>>>>> Mailing list:
>>>>>> https://launchpad.net/~kicad-devel
>>>>>> <https://launchpad.net/%7Ekicad-devel>
>>>>>>>>>>>> oper
>>>>>>>>>>>> s
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>>
>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>>
>>>>>>>>>>>> Post to :
>>>>>> kicad-developers@lists.launchpad.n
>>>>>>>>>>>> et
>>>>>>>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>>
>>>>>>>>>>>>
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>>>
>>>>>>>>>>>> Unsubscribe :
>>>>>> https://launchpad.net/~kicad-devel
>>>>>> <https://launchpad.net/%7Ekicad-devel>
>>>>>>>>>>>> oper
>>>>>>>>>>>> s
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>>
>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/%7Ekicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>>
>>>>>>>>>>>> More help :
>>>>>> https://help.launchpad.net/ListHel
>>>>>> <https://help.launchpad.net/ListHel>
>>>>>>>>>>>> p
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>>
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> _______________________________________________
>>>>>>>>>>>> Mailing list:
>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>> Post to :
>>>>>> kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>>
>>>>>>>>>>>> Unsubscribe :
>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> <https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>>
>>>>>>>>>>>> More help :
>>>>>> https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>>>> <https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> --
>>>>>>>>>>>> Remember The Past, Live The Present, Change The Future
>>>>>>>>>>>> Those who look only to the past or the present are
>>>>>> certain
>>>>>>>>>>>> to
>>>>>>>>>>>> miss
>>>>>>>>>>>> the
>>>>>>>>>>>> future [JFK]
>>>>>>>>>>>>
>>>>>>>>>>>> kandrey89@xxxxxxxxx <mailto:kandrey89@xxxxxxxxx>
>>>>>> <mailto:kandrey89@xxxxxxxxx <mailto:kandrey89@xxxxxxxxx>>
>>>>>>>>>>>> Live Long and Prosper,
>>>>>>>>>>>> Andrey
>>>>>>>>>>>>
>>>>>>>>>>>>
>>>>>>>>>>>> _______________________________________________
>>>>>>>>>>>> Mailing list:
>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>>>>>> Unsubscribe :
>>>>>> https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>>>>
>>>>>>>>>>>
>>>>>>>>>>> _______________________________________________
>>>>>>>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>>
>>>>>>>>>> <0001-Added-default-fields-not-affect-previous-
>>>>>>>>>>
>>>>>> designs.patch>_______________________________________________
>>>>>>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>>
>>>>>>>>>
>>>>>>>>
>>>>>>>> _______________________________________________
>>>>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>>>
>>>>>>>
>>>>>>>
>>>>>>
>>>>>> _______________________________________________
>>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>> <https://help.launchpad.net/ListHelp>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>> _______________________________________________
>>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>>> More help : https://help.launchpad.net/ListHelp
>>>>>
>>>>>
>>>>> _______________________________________________
>>>>> Mailing list: https://launchpad.net/~kicad-developers
>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>>>>> <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>>>>> Unsubscribe : https://launchpad.net/~kicad-developers
>>>>> <https://launchpad.net/%7Ekicad-developers>
>>>>> More help : https://help.launchpad.net/ListHelp
>>>>
>>>
>>
>>
>>
>> _______________________________________________
>> Mailing list: https://launchpad.net/~kicad-developers
>> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
>> Unsubscribe : https://launchpad.net/~kicad-developers
>> More help : https://help.launchpad.net/ListHelp
>>
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help : https://help.launchpad.net/ListHelp
Follow ups
References
-
More default fields in schematic
From: kristoffer Ödmark, 2018-05-20
-
Re: More default fields in schematic
From: Seth Hillbrand, 2018-05-20
-
Re: More default fields in schematic
From: Kristoffer Ödmark, 2018-05-20
-
Re: More default fields in schematic
From: José Ignacio, 2018-05-20
-
Re: More default fields in schematic
From: kristoffer Ödmark, 2018-05-20
-
Re: More default fields in schematic
From: Andrey Kuznetsov, 2018-05-20
-
Re: More default fields in schematic
From: Wayne Stambaugh, 2018-05-21
-
Re: More default fields in schematic
From: kristoffer ödmark, 2018-05-22
-
Re: More default fields in schematic
From: Jeff Young, 2018-05-22
-
Re: More default fields in schematic
From: kristoffer ödmark, 2018-05-22
-
Re: More default fields in schematic
From: Ben Hest, 2018-05-22
-
Re: More default fields in schematic
From: kristoffer ödmark, 2018-05-22
-
Re: More default fields in schematic
From: Fabrizio Tappero, 2018-05-22
-
Re: More default fields in schematic
From: Reece R. Pollack, 2018-05-28
-
Re: More default fields in schematic
From: Jeff Young, 2018-05-29
-
Re: More default fields in schematic
From: Reece R. Pollack, 2018-05-29
-
Re: More default fields in schematic
From: Jeff Young, 2018-05-29
-
Re: More default fields in schematic
From: Wayne Stambaugh, 2018-05-29
