gEDA-user: updating layout with new footprint

[Ostheller, Joel A.]

Some parts of this message have been removed. Learn more about Nabble's security policy.

I finished a layout, but decided that I really should change one of my footprints. Is there a way to update my .pcb for all updated footprints without having to redo placement and hand routing?

_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> I finished a layout, but decided that I really should change one of my
> footprints. Is there a way to update my .pcb for all updated footprints
> without having to redo placement and hand routing?

Not quite.  What you can do is use shift-click to replace a footprint
with a new one (rather than regular click to place a second footprint
on top of the old one) but we have no automated way of doing it.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Ostheller, Joel A.]

Can you please explain this shit click technique a little more?

> -----Original Message-----
> From: geda-user-bounces@... [mailto:geda-user-
> bounces@...] On Behalf Of DJ Delorie
> Sent: Tuesday, January 09, 2007 12:42 PM
> To: geda-user@...
> Subject: Re: gEDA-user: updating layout with new footprint
>
>
> > I finished a layout, but decided that I really should change one of
my
> > footprints. Is there a way to update my .pcb for all updated
footprints

> > without having to redo placement and hand routing?
>
> Not quite.  What you can do is use shift-click to replace a footprint
> with a new one (rather than regular click to place a second footprint
> on top of the old one) but we have no automated way of doing it.
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@...
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> Can you please explain this shift click technique a little more?

You need to be more careful about your spelling.

Shift-click is when you hold the shift key while clicking with the
left mouse button.

Specifically, use the Info->Library dialog box to manually choose the
new footprint.  The tool becomes the buffer-paste tool, with the new
footprint preloaded.  Rotate it if needed with Buffer->Rotate Buffer.
Position the new footprint over the old one, and
shift-left-mouse-click to replace the old footprint with the new one.
Watch out for being 180 degrees off, use 'o' to check the rats nest
after each placement, and undo if it appears you placed it backwards.

Note that this is the same technique used to manually place parts,
except the shift key causes it to replace the footprint instead of
placing a new one.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[John Griessen]

DJ Delorie wrote:

> Position the new footprint over the old one, and
> shift-left-mouse-click to replace the old footprint with the new one.
> Watch out for being 180 degrees off, use 'o' to check the rats nest
> after each placement, and undo if it appears you placed it backwards.
>

Do you position it to exact grid snap position, or less precise?

John G


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> Do you position it to exact grid snap position, or less precise?

I keep a standard grid on when placing parts, so I can replace them
accurately.

But you end up positioning the crosshairs on the old element's mark
anyway, so it's not that hard to be accurate enough.

At least, as long as you don't move the mark, or the pads ;-)


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Ostheller, Joel A.]

DJ - Thank you for all the help you have been today; I have learned a
lot about geda.

I am still having difficulty with the Shift-click technique for part
replacement. I am running PCB 20060822. I do not have an Info->Library
dialog box, but I do have a Window->Library Dialog box. When I
origionally made this PCB, I had created a footprint called "foobar". I
have recently gone back and update "foobar" with a more accurate
footprint (bigger pads, more ground vias). Thus the old "foobar" no
longer exists except in my PCB design. I am trying to replace that old
footprint with the new one that exists.

When I select this newlib footprint "foobar" from the Window->Library I
can manually place it anywhere with a left mouse click. If I hold down
the shift key and left mouse click on the old "foobar" footprint, then
it just puts a new footprint over the old footprint.

What am I doing wrong?

> -----Original Message-----
> From: geda-user-bounces@... [mailto:geda-user-
> bounces@...] On Behalf Of DJ Delorie
> Sent: Tuesday, January 09, 2007 3:04 PM
> To: geda-user@...
> Subject: Re: gEDA-user: updating layout with new footprint
>
>
> > Can you please explain this shift click technique a little more?
>
> You need to be more careful about your spelling.
>
> Shift-click is when you hold the shift key while clicking with the
> left mouse button.
>
> Specifically, use the Info->Library dialog box to manually choose the
> new footprint.  The tool becomes the buffer-paste tool, with the new
> footprint preloaded.  Rotate it if needed with Buffer->Rotate Buffer.
> Position the new footprint over the old one, and
> shift-left-mouse-click to replace the old footprint with the new one.
> Watch out for being 180 degrees off, use 'o' to check the rats nest
> after each placement, and undo if it appears you placed it backwards.
>
> Note that this is the same technique used to manually place parts,
> except the shift key causes it to replace the footprint instead of
> placing a new one.
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@...
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Ostheller, Joel A.]

Ahhh... So if I move the mark then I am in a guessing game =) great

> -----Original Message-----
> From: geda-user-bounces@... [mailto:geda-user-
> bounces@...] On Behalf Of DJ Delorie
> Sent: Tuesday, January 09, 2007 4:07 PM
> To: john_g@...; geda-user@...
> Subject: Re: gEDA-user: updating layout with new footprint
>
>
> > Do you position it to exact grid snap position, or less precise?
>
> I keep a standard grid on when placing parts, so I can replace them
> accurately.
>
> But you end up positioning the crosshairs on the old element's mark
> anyway, so it's not that hard to be accurate enough.
>
> At least, as long as you don't move the mark, or the pads ;-)
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@...
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> I am still having difficulty with the Shift-click technique for part
> replacement. I am running PCB 20060822.

Too old.  I added that in September.

> I do not have an Info->Library dialog box, but I do have a
> Window->Library Dialog box.

Same thing, different GUI.

> Thus the old "foobar" no longer exists except in my PCB design.

Right.  You're replacing the footprint on the board with a new one.

> When I select this newlib footprint "foobar" from the Window->Library I
> can manually place it anywhere with a left mouse click. If I hold down
> the shift key and left mouse click on the old "foobar" footprint, then
> it just puts a new footprint over the old footprint.

You need a newer pcb; perhaps CVS.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> Ahhh... So if I move the mark then I am in a guessing game =) great

Yup, but it's not that hard to line them up manually.

It's a lot harder if you have to delete the old element first, because
you no longer have a reference.  Plus, the shift-click feature copies
the refdes, value, and description from the old to the new for you.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Kai-Martin Knaak]

On Tue, 09 Jan 2007 18:04:15 -0500, DJ Delorie wrote:

> Specifically, use the Info->Library dialog box to manually choose the
> new footprint.  The tool becomes the buffer-paste tool, with the new
> footprint preloaded.  Rotate it if needed with Buffer->Rotate Buffer.
> Position the new footprint over the old one, and
> shift-left-mouse-click to replace the old footprint with the new one.
> Watch out for being 180 degrees off, use 'o' to check the rats nest
> after each placement, and undo if it appears you placed it backwards.

Thanks, this is a non obvious hint. I used these lines to add a hint to the
wiki:
http://geda.seul.org/wiki/geda:pcb_tips#how_do_i_add_a_footprint_library_to_pcb

---<(kaimartin)>---
--
Kai-Martin Knaak
http://lilalaser.de/blog



_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[joe tarantino]

Ostheller, Joel A. wrote:

> I finished a layout, but decided that I really should change one of my
> footprints. Is there a way to update my .pcb for all updated
> footprints without having to redo placement and hand routing? //
>
>  
>
A while back David Rowe posted a perl script to this list to
automatically update footprints in a PCB file.  I added a couple very
minor tweaks to work with the part building conventions I use.  The
algorithm is fairly simple-minded, but I've used it with good success on
several occasions.

I can send it to you if you are interested.  No guarantees.

Thanks again to David for making this tool available in the first place.

Joe T

>
>_______________________________________________
>geda-user mailing list
>geda-user@...
>http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
>  
>



_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[drowe67]

> Thanks again to David for making this tool available in the first place.

You are very welcome Joe.  There is a page on this tool here:
http://www.rowetel.com/perl4pcb.html

Joe - pls contact me off list, lets finish off those mods to this tool
that u submitted.

- David

>
> Joe T
>
> >
> >_______________________________________________
> >geda-user mailing list
> >geda-user@...
> >http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
> >  
> >
>
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@...
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Levente Kovacs-2]

On Fri, 12 Jan 2007 06:38:43 +1030
David Rowe <david@...> wrote:

> Joe - pls contact me off list, lets finish off those mods to this tool
> that u submitted.

Could you please post your changes to the list please... Thank you.

Levente



_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Simon_T]

When i try to update elements with the shift-left-mouse-click my PCB program crashes.
I have a 20070208 version.

Any one ?

grtz

Simon

DJ Delorie wrote:

> I finished a layout, but decided that I really should change one of my
> footprints. Is there a way to update my .pcb for all updated footprints
> without having to redo placement and hand routing?

Not quite.  What you can do is use shift-click to replace a footprint
with a new one (rather than regular click to place a second footprint
on top of the old one) but we have no automated way of doing it.


_______________________________________________
geda-user mailing list
[e-mail]
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> When i try to update elements with the shift-left-mouse-click my PCB
> program crashes.

1. lesstif or gtk?

2. Could you try cvs to see if it's fixed?

3. Could you run pcb under gdb, and type "where" when it crashes?

Otherwise, this works for me.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[ST de Feber]

>>1. lesstif or gtk?
[ST : GTK.
I am running slackware 10.2


>>2. Could you try cvs to see if it's fixed?
[ST : i am not fimilar with CVS.
Is there a help on howto retrieve new code ?

>>3. Could you run pcb under gdb, and type "where" when it crashes?
[ST : It took me a few minutes te figure out how to run gdb with PCB, but here it is !

Program received signal SIGSEGV, Segmentation fault.
backN_callback (b=0x827abf8, cl=0x0) at draw.c:318
318       if (!FRONT (element) && !TEST_FLAG (HIDENAMEFLAG, element))
(gdb) where
#0  backN_callback (b=0x827abf8, cl=0x0) at draw.c:318
#1  0x080ab4f6 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:594
#2  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#3  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#4  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#5  0x080ab6af in r_search (rtree=0x0, query=0x827abf8, check_region=0, found_rectangle=0x807bdf0 <backN_callback>,
    cl=0x0) at rtree.c:626
#6  0x0807cb29 in DrawEverything (drawn_area=0xbfffecb0) at draw.c:487
#7  0x080802cc in hid_expose_callback (hid=0x80f9320, region=0xbfffecb0, item=0xbfffecb0) at draw.c:2517
#8  0x080bba0d in ghid_invalidate_all () at hid/gtk/gtkhid-main.c:260
#9  0x0807bd0b in Draw () at draw.c:199
#10 0x080a75c5 in RemoveElement (Element=0x827aba0) at remove.c:524
#11 0x0805a38c in NotifyMode () at action.c:1379
#12 0x0805c7c6 in ActionMode (argc=1, argv=0x827abf8, x=0, y=0) at action.c:2947
#13 0x080b8844 in hid_actionv (name=0x80da2f1 "Mode", argc=1, argv=0xbfffeef0) at hid/common/actions.c:216
#14 0x080b87df in hid_actionl (name=0x80da2f1 "Mode") at hid/common/actions.c:194
#15 0x080c508a in ghid_port_button_press_cb (drawing_area=0x8308aa0, ev=0x8164cb8, ui=0x8203e40)
    at hid/gtk/gui-output-events.c:996
#16 0x401804b0 in gtk_marshal_VOID__UINT_STRING () from /usr/lib/libgtk-x11-2.0.so.0
#17 0x40486215 in g_closure_invoke () from /usr/lib/libgobject-2.0.so.0
#18 0x40497e6f in signal_emit_unlocked_R () from /usr/lib/libgobject-2.0.so.0
#19 0x40496d1a in g_signal_emit_valist () from /usr/lib/libgobject-2.0.so.0
#20 0x404971c6 in g_signal_emit () from /usr/lib/libgobject-2.0.so.0
#21 0x40276f67 in gtk_widget_send_expose () from /usr/lib/libgtk-x11-2.0.so.0
#22 0x4017ef82 in gtk_propagate_event () from /usr/lib/libgtk-x11-2.0.so.0
#23 0x4017ddc6 in gtk_main_do_event () from /usr/lib/libgtk-x11-2.0.so.0
#24 0x403854b5 in gdk_x11_register_standard_event_type () from /usr/lib/libgdk-x11-2.0.so.0
#25 0x404dad82 in g_main_dispatch () from /usr/lib/libglib-2.0.so.0
#26 0x404dbdf8 in g_main_context_dispatch () from /usr/lib/libglib-2.0.so.0
#27 0x404dc130 in g_main_context_iterate () from /usr/lib/libglib-2.0.so.0
#28 0x404dc6d3 in g_main_loop_run () from /usr/lib/libglib-2.0.so.0
#29 0x4017d673 in gtk_main () from /usr/lib/libgtk-x11-2.0.so.0
#30 0x080cb9b9 in ghid_do_export (options=0x0) at hid/gtk/gui-top-window.c:3850
#31 0x0808fd95 in main (argc=2, argv=0xbffff5d4) at main.c:992



----- Original Message ----
From: DJ Delorie <dj@...>
To: geda-user@...
Sent: Monday, 13 August, 2007 1:02:18 PM
Subject: Re: gEDA-user: updating layout with new footprint


> When i try to update elements with the shift-left-mouse-click my PCB
> program crashes.

1. lesstif or gtk?

2. Could you try cvs to see if it's fixed?

3. Could you run pcb under gdb, and type "where" when it crashes?

Otherwise, this works for me.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user





      ___________________________________________________________
Yahoo! Answers - Got a question? Someone out there knows the answer. Try it
now.
http://uk.answers.yahoo.com/ 


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[ST de Feber]

DJ (and Others),

I found on your website a description on howto get the CVS code !
Should i get everything and recompile or replace parts of the code and then recompile?

grtz

Simon


----- Original Message ----
From: ST de Feber <stdf23173@...>
To: gEDA user mailing list <geda-user@...>
Sent: Monday, 13 August, 2007 7:14:33 PM
Subject: Re: gEDA-user: updating layout with new footprint

>>1. lesstif or gtk?
[ST : GTK.
I am running slackware 10.2


>>2. Could you try cvs to see if it's fixed?
[ST : i am not fimilar with CVS.
Is there a help on howto retrieve new code ?

>>3. Could you run pcb under gdb, and type "where" when it crashes?
[ST : It took me a few minutes te figure out how to run gdb with PCB, but here it is !

Program received signal SIGSEGV, Segmentation fault.
backN_callback (b=0x827abf8, cl=0x0) at draw.c:318
318       if (!FRONT (element) && !TEST_FLAG (HIDENAMEFLAG, element))
(gdb) where
#0  backN_callback (b=0x827abf8, cl=0x0) at draw.c:318
#1  0x080ab4f6 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:594
#2  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#3  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#4  0x080ab630 in __r_search (node=0x827abf8, query=0xbfffecb0, arg=0xbfffeb20) at rtree.c:590
#5  0x080ab6af in r_search (rtree=0x0, query=0x827abf8, check_region=0, found_rectangle=0x807bdf0 <backN_callback>,
    cl=0x0) at rtree.c:626
#6  0x0807cb29 in DrawEverything (drawn_area=0xbfffecb0) at draw.c:487
#7  0x080802cc in hid_expose_callback (hid=0x80f9320, region=0xbfffecb0, item=0xbfffecb0) at draw.c:2517
#8  0x080bba0d in ghid_invalidate_all () at hid/gtk/gtkhid-main.c:260
#9  0x0807bd0b in Draw () at draw.c:199
#10 0x080a75c5 in RemoveElement (Element=0x827aba0) at remove.c:524
#11 0x0805a38c in NotifyMode () at action.c:1379
#12 0x0805c7c6 in ActionMode (argc=1, argv=0x827abf8, x=0, y=0) at action.c:2947
#13 0x080b8844 in hid_actionv (name=0x80da2f1 "Mode", argc=1, argv=0xbfffeef0) at hid/common/actions.c:216
#14 0x080b87df in hid_actionl (name=0x80da2f1 "Mode") at hid/common/actions.c:194
#15 0x080c508a in ghid_port_button_press_cb (drawing_area=0x8308aa0, ev=0x8164cb8, ui=0x8203e40)
    at hid/gtk/gui-output-events.c:996
#16 0x401804b0 in gtk_marshal_VOID__UINT_STRING () from /usr/lib/libgtk-x11-2.0.so.0
#17 0x40486215 in g_closure_invoke () from /usr/lib/libgobject-2.0.so.0
#18 0x40497e6f in signal_emit_unlocked_R () from /usr/lib/libgobject-2.0.so.0
#19 0x40496d1a in g_signal_emit_valist () from /usr/lib/libgobject-2.0.so.0
#20 0x404971c6 in g_signal_emit () from /usr/lib/libgobject-2.0.so.0
#21 0x40276f67 in gtk_widget_send_expose () from /usr/lib/libgtk-x11-2.0.so.0
#22 0x4017ef82 in gtk_propagate_event () from /usr/lib/libgtk-x11-2.0.so.0
#23 0x4017ddc6 in gtk_main_do_event () from /usr/lib/libgtk-x11-2.0.so.0
#24 0x403854b5 in gdk_x11_register_standard_event_type () from /usr/lib/libgdk-x11-2.0.so.0
#25 0x404dad82 in g_main_dispatch () from /usr/lib/libglib-2.0.so.0
#26 0x404dbdf8 in g_main_context_dispatch () from /usr/lib/libglib-2.0.so.0
#27 0x404dc130 in g_main_context_iterate () from /usr/lib/libglib-2.0.so.0
#28 0x404dc6d3 in g_main_loop_run () from /usr/lib/libglib-2.0.so.0
#29 0x4017d673 in gtk_main () from /usr/lib/libgtk-x11-2.0.so.0
#30 0x080cb9b9 in ghid_do_export (options=0x0) at hid/gtk/gui-top-window.c:3850
#31 0x0808fd95 in main (argc=2, argv=0xbffff5d4) at main.c:992



----- Original Message ----
From: DJ Delorie <dj@...>
To: geda-user@...
Sent: Monday, 13 August, 2007 1:02:18 PM
Subject: Re: gEDA-user: updating layout with new footprint


> When i try to update elements with the shift-left-mouse-click my PCB
> program crashes.

1. lesstif or gtk?

2. Could you try cvs to see if it's fixed?

3. Could you run pcb under gdb, and type "where" when it crashes?

Otherwise, this works for me.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user





      ___________________________________________________________
Yahoo! Answers - Got a question? Someone out there knows the answer. Try it
now.
http://uk.answers.yahoo.com/ 


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user





      ___________________________________________________________
Yahoo! Answers - Got a question? Someone out there knows the answer. Try it
now.
http://uk.answers.yahoo.com/ 


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[Peter Clifton-2]

On Wed, 2007-08-15 at 11:01 +0000, ST de Feber wrote:
>
> I found on your website a description on howto get the CVS code !
> Should i get everything and recompile or replace parts of the code and
> then recompile?

I think the suggestion was to grab everything (the PCB sources anyway),
and compile that unchanged. If the new version of PCB fixes the bug
you're seeing then we're sorted. If not, there will probably be further
debugging needed.

Regards,

--
Peter Clifton

Electrical Engineering Division,
Engineering Department,
University of Cambridge,
9, JJ Thomson Avenue,
Cambridge
CB3 0FA

Tel: [phone] - (No signal in the lab!)



_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user

[DJ Delorie]

> Should i get everything and recompile or replace parts of the code
> and then recompile?

Get the whole pcb module and build it.  You can run the "pcb"
executable directly from src/pcb, you don't have to install anything
to test it.


_______________________________________________
geda-user mailing list
geda-user@...
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user