[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]
Re: gEDA-user: Error in Centroid Calculation
Hello Bert,
The description of the problem in the Jan-2008 message sounds exactly
like the problem that is in the 20080202 version. Maybe I should try the CVS
version. I downloaded the 20080202 tarball yesterday.
The 2005xxxx version gives the correct centroid or may just default to the
value of the mark which happens to be the correct centroid for this footprint.
Thanks for the information.
(* jcl *)
On Mon, Sep 29, 2008 at 3:26 PM, Bert Timmerman
<bert.timmerman@xxxxxxxxx> wrote:
> Hi John,
>
> In my git-ified pcb repo I have:
> <quote>
> Author: danmc <danmc>
> Date: 01/03/2008 12:45:12 AM
> Parent: change the preprocessor logic a bit to avoid #ifdef-ing i...
> Child: apply patch 1852864 GTK HID: scrolled layer preferences
> Branch: master (Display nets as a hierarchical tree in the netlist
> window.) origin (Display nets as a hierarchical tree in the netlist
> window.)
> Branch: pcb-20080202 (set version for 20080202 release)
> Follows: pcb-20070912-base (news for 20070912)
> Precedes: pcb-20080202-base (update for 20080202)
>
> Fix a problem with the X-Y output file where the y values were mirrored
> and offset with respect to the RS274-X output. Given that this bug has
> been here since the code was written 3 years ago, I conclude that in
> fact no one has used this feature.
> </quote>
>
> also look at:
>
> http://archives.seul.org/geda/user/Jan-2008/msg00016.html
>
> Kind regards,
>
> Bert Timmerman.
>
> On Mon, 2008-09-29 at 13:04 -0400, John Luciani wrote:
>> IIRC board coordinates are measured from the upper left
>> so board size should have no affect on the centroid coordinates
>> within my board.
>>
>> If I center the crosshair in the center of the 0805 (which is the
>> centroid for this package) both versions of PCB display
>> the value (700,325). When the xy data is output the two versions
>> differ.
>>
>> (* jcl *)
>>
>> On Mon, Sep 29, 2008 at 12:04 PM, Bert Timmerman
>> <bert.timmerman@xxxxxxxxx> wrote:
>> > Hmm, let's do some math:
>> >
>> > Board size: Xpcb = 184200, Ypcb = 85400 [mil/100].
>> >
>> > C1 is on: Xcomp = 700, Ycomp = 325 [mil]
>> >
>> > Centroid XY coords: X = Xcomp, Y = Ypcb - Ycomp = 854 -325 = 529 [mil]
>> >
>> > Hmm, version 20080202 looks good to me.
>> >
>> > Where are your origins ?
>> >
>> > IIRC, Dan did explain this one (and complain about nobody using this
>> > feature, since he found it was buggy for years !).
>> >
>> > Kind regards,
>> >
>> > Bert Timmerman.
>> >
>> > On Mon, 2008-09-29 at 09:13 -0400, John Luciani wrote:
>> >> There appears to be an error in the centroid calculation in
>> >> pcb-20080202. If I load the pcb (below) in version pcb-20050315 and
>> >> output the xy data I get
>> >>
>> >> C1,"0805","0.1u",700.00,325.00,0,bottom
>> >>
>> >> when I output xy data with pcb-20080202 (both lesstif and gtk)
>> >> I get
>> >>
>> >> C1,"0805","0.1u",700.00,529.00,0,bottom
>> >>
>> >> For this footprint the mark is set at the centroid. (700,325) is
>> >> correct.
>> >>
>> >> (* jcl *)
>> >>
>> >> #-------- pcb example -----------
>> >>
>> >> # release: pcb-bin 20050315
>> >> # date: Mon Sep 29 08:04:13 2008
>> >> # user: jluciani (jluciani)
>> >> # host: rossini.luciani-family.org
>> >>
>> >> PCB["" 184200 85400]
>> >>
>> >> Grid[2500.00000000 0 0 1]
>> >> Cursor[171354 117519 2.391741]
>> >> Thermal[0.500000]
>> >> DRC[749 10 800 800]
>> >> Flags(0x00000000000018d8)
>> >> Groups("1,c:2,s:3:4:5:6:7:8")
>> >> Styles["Signal,1200,3800,2000,1000:Power,2500,6500,4600,1000:Fat,5000,7500,5200,1000:Skinny,900,3200,1600,1000"]
>> >>
>> >> Element[0x00000080 "0805" "C1" "0.1u" 70000 32500 14799 -2421 2 100 0x00000080]
>> >> (
>> >> Pad[-3740 -393 -3740 393 5118 2000 6118 "input" "1" 0x00000180]
>> >> Pad[3740 -393 3740 393 5118 2000 6118 "input" "2" 0x00000180]
>> >> ElementLine [-7799 -4452 7799 -4452 1000]
>> >> ElementLine [7799 -4452 7799 4452 1000]
>> >> ElementLine [-7799 4452 7799 4452 1000]
>> >> ElementLine [-7799 -4452 -7799 4452 1000]
>> >>
>> >> )
>> >>
>> >> Layer(1 "component")
>> >> (
>> >> )
>> >> Layer(2 "solder")
>> >> (
>> >> )
>> >> Layer(3 "3")
>> >> (
>> >> )
>> >> Layer(4 "4")
>> >> (
>> >> )
>> >> Layer(5 "5")
>> >> (
>> >> )
>> >> Layer(6 "6")
>> >> (
>> >> )
>> >> Layer(7 "7")
>> >> (
>> >> )
>> >> Layer(8 "outline")
>> >> (
>> >> )
>> >> Layer(9 "silk")
>> >> (
>> >> )
>> >> Layer(10 "silk")
>> >> (
>> >> )
>> >> NetList()
>> >> (
>> >> )
>> >>
>> >>
>> >
>> >
>> >
>> > _______________________________________________
>> > geda-user mailing list
>> > geda-user@xxxxxxxxxxxxxx
>> > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
>> >
>>
>>
>>
>
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@xxxxxxxxxxxxxx
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
>
--
http://www.luciani.org
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user