kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxx>]

Looks good to me.  If no one else objects, I see no reason not not to
merge it.

Wayne

On 7/5/19 12:25 PM, Jeff Young wrote:
> Oops.  Good catch.
> 
>> On 5 Jul 2019, at 16:43, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
>>
>> Looks good to me.  Thanks Jeff!  The only thing that I didn't see was the file version bump.
>>
>> Let's see if anyone else want to weigh in after this thread :)
>>
>> -Seth
>>
>> On 2019-07-05 09:46, Jeff Young wrote:
>>> Git is alive again:
>>> https://git.launchpad.net/~jeyjey/kicad/commit/?id=602bd05291677de97e50e84bef7a3510ff80be23
>>>> On 5 Jul 2019, at 12:19, Jeff Young <jeff@xxxxxxxxx> wrote:
>>>> (setup
>>>> (last_trace_width 0.25)
>>>> (trace_clearance 0.2)
>>>> (zone_clearance 0.508)
>>>> (zone_45_only no)
>>>> (trace_min 0.2)
>>>> (via_size 0.8)
>>>> (via_drill 0.4)
>>>> (via_min_size 0.4)
>>>> (via_min_drill 0.3)
>>>> (user_diff_pair 1 2 3)
>>>> (uvia_size 0.3)
>>>> (uvia_drill 0.1)
>>>> (uvias_allowed no)
>>>> (uvia_min_size 0.2)
>>>> (uvia_min_drill 0.1)
>>>> (max_error 0.005)
>>>> (defaults
>>>> (edge_clearance 0.01)
>>>> (edge_cuts_line_width 0.05)
>>>> (courtyard_line_width 0.05)
>>>> (copper_line_width 0.2)
>>>> (copper_text_dims (size 1.5 1.5) (thickness 0.3) keep_upright)
>>>> (silk_line_width 0.12)
>>>> (silk_text_dims (size 1 1) (thickness 0.15) keep_upright)
>>>> (other_layers_line_width 0.1)
>>>> (other_layers_text_dims (size 1 1) (thickness 0.15)
>>>> keep_upright)
>>>> )
>>>> (pad_size 1.524 1.524)
>>>> (pad_drill 0.762)
>>>> (pad_to_mask_clearance 0.051)
>>>> (solder_mask_min_width 0.25)
>>>> (aux_axis_origin 0 0)
>>>> (visible_elements FEFFFF7F)
>>>> (pcbplotparams
>>>> (layerselection 0x01000_7fffffff)
>>>> (usegerberextensions false)
>>>> (usegerberattributes false)
>>>> (usegerberadvancedattributes false)
>>>> (creategerberjobfile false)
>>>> (excludeedgelayer true)
>>>> (linewidth 0.101600)
>>>> (plotframeref false)
>>>> (viasonmask false)
>>>> (mode 1)
>>>> (useauxorigin false)
>>>> (hpglpennumber 1)
>>>> (hpglpenspeed 20)
>>>> (hpglpendiameter 15.000000)
>>>> (psnegative false)
>>>> (psa4output false)
>>>> (plotreference true)
>>>> (plotvalue true)
>>>> (plotinvisibletext false)
>>>> (padsonsilk false)
>>>> (subtractmaskfromsilk false)
>>>> (outputformat 5)
>>>> (mirror false)
>>>> (drillshape 0)
>>>> (scaleselection 1)
>>>> (outputdirectory ""))
>>>> )
>>>> Good to go?
>>>> Cheers,
>>>> Jeff.
>>>> (I can post the code later, but our git instance seems to be down.)
>>>> On 5 Jul 2019, at 02:32, hauptmech <hauptmech@xxxxxxxxx> wrote:
>>>> Not requiring DR/DRC is appreciated.
>>>> Netclasses don't work with my designs on a fundamental level and if
>>>> there were not a way I could ignore them, I would not be able to use
>>>> KiCAD. Likewise the new interactive router which spends most of its
>>>> time in Highlight Collisions mode with Allow DRC Violations. I use
>>>> it normally when I can, but that's not very often.
>>>> The knowledge of the kicad developers of leading edge and specialist
>>>> board design has consistently been limited and if you bake in that
>>>> limited knowledge into DR/DRC with no fallback, you will shoot some
>>>> users in the foot.
>>>> It doesn't need to be the old system but it does need to be free of
>>>> assumptions about what is acceptable data for the manufacturer and
>>>> what is acceptable practice for the designer.
>>>> On 5/07/2019 11:45 AM, Jeff Young wrote:
>>>> Hi Seth,
>>>> I was thinking about a similar issue which is that we probably
>>>> can’t require users to move to the new DR system (as it will be
>>>> considerably more technical).  So perhaps using the old system as
>>>> defaults which can be overridden by the new makes sense.
>>>> Cheers,
>>>> Jeff.
>>>> On 4 Jul 2019, at 22:40, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
>>>> Hi Jeff-
>>>> Ideally, I'd like to find an option that doesn't need to move twice
>>>> during v6.  Toward that goal, what if we moved edge_clearance to the
>>>> defaults section?  Until we implement the design rules and/or
>>>> polygon-specific clearance, it simply controls everything.  Once we
>>>> integrate the new features, they are allowed to override the
>>>> default.
>>>> Thoughts?
>>>> -Seth
>>>> On 2019-07-04 12:07, Jeff Young wrote:
>>>> Looking through our current set of board setup properties, only
>>>> solder_mask_min_width would join edge_clearance in a design_rules
>>>> section.
>>>> Most of the other properties are either most-recently-used values
>>>> (zone_clearance, via_size, etc.) or true DRC values (uvias_allowed,
>>>> trace_min, etc.).
>>>> The outlier is max_error, which is mostly a performance vs beauty
>>>> trade-off, but _does_ affect the generated board.
>>>> So,
>>>> 1) leave solder_mask_min_width and edge_clearance in setup for now
>>>> 2) create a design_rules section for solder_mask_min_width and
>>>> edge_clearance
>>>> 3) leave edge_clearance in the project file for now
>>>> I think I’d vote for (1) simply because I don’t know how (2)
>>>> will
>>>> play with Jon’s stuff.  But the only one I don’t like is (3).
>>>> Cheers,
>>>> Jeff.
>>>> On 4 Jul 2019, at 15:42, Seth Hillbrand <seth@xxxxxxxxxxxxx> wrote:
>>>> On 2019-07-04 09:24, Jeff Young wrote:
>>>> Since this is DRC, can we keep it in its current place until the DRC
>>>> manager goes in
>>>> Well, there’s DRC and there’s DR.  The other options really
>>>> control
>>>> only what is *checked*, whereas this one controls stuff *on* the
>>>> board.  Granted a lot of Jon’s rules will also fit into the DR
>>>> camp,
>>>> but I feel a little more reticent to move this one out.
>>>> Thoughts?
>>>> Jeff.
>>>> That's a valid point.  Ideally, I'd like to see this in a
>>>> "DesignRules" section.  Different manufacturers will have different
>>>> requirements here, so the DRC/DFM import would need to modify this
>>>> value.  The check also needs to allow separate values for internal
>>>> vs.
>>>> external layers.
>>>> If we want to separate the generation from the checking, we might
>>>> want
>>>> to put this setting in the zone parameters.  In which case, we might
>>>> use a global default setting that is used for new zones.
>>>> -Seth
>>> _______________________________________________
>>> 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
>>> _______________________________________________
>>> 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
> 
> 
> _______________________________________________
> 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
>