gEDA-user: Symbol creation
Hi! The included symbol looses its attributes when opened in a gschem window (when I look at main menue EDIT/EDIT) with some other symbols. The symbols from the default libraries do not loose its attributes. Thank you for your kindly treatment to my newbie problems. ostene pgnd-1.sym Description: application/geda-symbol ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: improved footprint for MSOP10
Hi, since the library version footprint MSOP10.fp seems to be very unprecise, I made my own, which is included below. The major difference is in the spacing of pads. Regards, Armin MSOP10_ajf.fp Description: application/pcb-footprint ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: improved footprint for MSOP10
On Fri, 2010-09-24 at 13:01 +0200, Armin Faltl wrote: Hi, since the library version footprint MSOP10.fp seems to be very unprecise, I made my own, which is included below. The major difference is in the spacing of pads. Regards, Armin very unprecise, Please try to give more detailed error reports -- if that one is really wrong, we should remove it. To yours: Do you really think that it is a good idea to have the text overlapping the pads by default position? The silk is close to the pads on the left and right side, at least distance is not symmetric on all four sides. Please note, it is a good idea to specify source of layout data and license for distribution. PCB footprints can have attributes for that. Hexadecimal flags may be OK, but textual ones seems to be preferred in these days. Is is really useful to have these thin soldermask areas between pads, or should we prefer a gang solder mask? This is a question, I am not sure, but I think there is no real advantage for these stripes, but manufactures can have problems with it -- ok I think they remove it anyway. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
On Fri, 2010-09-24 at 12:30 +0200, Östen Einarsson wrote: Hi! The included symbol looses its attributes when opened in a gschem window (when I look at main menue EDIT/EDIT) with some other symbols. The symbols from the default libraries do not loose its attributes. Thank you for your kindly treatment to my newbie problems. ostene That is NOT a symbol for gschem/gEDA. That file contains a pin, some lines... There is no line starting with C which is the beginning of a Symbol/Component. See http://geda.seul.org/wiki/geda:file_format_spec#component For making symbols I prefer tools like tragesym or djboxsym or similar, these tools give you fine symbols, which can be modified/tuned by gschem. Making new symbols from scratch with gschem may be difficult, I have never done that. 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: Symbol creation
Stefan Salewski wrote: That is NOT a symbol for gschem/gEDA. That file contains a pin, some lines... There is no line starting with C which is the beginning of a Symbol/Component. Sorry, that was nonsense, the lines starting with C belongs in the schematic files, not in the sym files. I am still learning the gEDA file format... But my recommendation using tragesym or djboxsym still holds. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
On Fri, 2010-09-24 at 14:22 +0200, Stefan Salewski wrote:
Stefan Salewski wrote:
That is NOT a symbol for gschem/gEDA.
That file contains a pin, some lines...
There is no line starting with C which is the beginning of a
Symbol/Component.
Sorry, that was nonsense, the lines starting with C belongs in the
schematic files, not in the sym files. I am still learning the gEDA file
format...
But my recommendation using tragesym or djboxsym still holds.
If we compare yours with lm741-1.sym we see that you have refdes inside
of pin, but it should be outside.
ste...@amd64x2 ~ $ cat /usr/share/gEDA/sym/linear/lm741-1.sym attachment.sym
v 20031231 1
T 625 950 8 8 0 0 0 0 1
device=LM741
T 225 350 9 8 1 0 0 0 1
LM741
T 200 900 8 10 1 1 0 0 1
refdes=U?
P 200 200 0 200 1 0 1
{
T 50 225 5 8 1 1 0 0 1
pinnumber=2
T 50 225 5 8 0 0 0 0 1
pinseq=2
}
P 200 600 0 600 1 0 1
{
T 50 625 5 8 1 1 0 0 1
pinnumber=3
T 50 625 5 8 0 0 0 0 1
pinseq=3
}
P 500 200 500 0 1 0 1
{
T 525 50 5 8 1 1 0 0 1
pinnumber=4
T 525 50 5 8 0 0 0 0 1
pinseq=4
}
P 800 400 1000 400 1 0 1
{
T 875 425 5 8 1 1 0 0 1
pinnumber=6
T 875 425 5 8 0 0 0 0 1
pinseq=6
}
P 500 600 500 800 1 0 1
{
T 550 675 5 8 1 1 0 0 1
pinnumber=7
T 550 675 5 8 0 0 0 0 1
pinseq=7
}
L 200 800 200 0 3 0 0 0 -1 -1
L 800 400 200 800 3 0 0 0 -1 -1
L 300 650 300 550 3 0 0 0 -1 -1
L 250 600 350 600 3 0 0 0 -1 -1
L 250 200 350 200 3 0 0 0 -1 -1
L 800 400 200 0 3 0 0 0 -1 -1
v 20091004 2
L 400 800 1000 800 3 0 0 0 -1 -1
L 500 700 900 700 3 0 0 0 -1 -1
L 600 600 800 600 3 0 0 0 -1 -1
P 700 1100 700 800 1 0 0
{
T 700 1100 5 10 0 0 0 0 1
pintype=pwr
T 505 500 5 10 0 1 180 6 1
pinlabel=PGND
T 605 1050 5 10 1 1 180 0 1
pinnumber=1
T 700 1100 5 10 0 0 0 0 1
pinseq=1
T 400 400 5 10 1 1 0 0 1
device=PGND
T 600 1200 5 10 1 1 0 0 1
refdes=P?
}
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
Östen Einarsson wrote:
The included symbol looses its attributes when opened
in a gschem window (when I look at main menue EDIT/EDIT)
with some other symbols.
All attributes in your pgnd.sym file, are associated with the pin. They are
within the pin environment given by curly brackets. Probably they got there
because you selected the pin, typed EE and added the attributes in the
attribute editor. In a sense, your symbol does not loose attributes, but
does not contain any, in the first place.
Attributes of the whole symbol should reside outside any environment. Use
the action Add_Attribute from the Add menu to add them to the symbol.
Shortcut is aa.
Some more notes on your symbol:
* A power symbol needs a net attribute to work as expected.
In your case, it should probably be
net=PGND:1
* A refdes attribute on a power symbol does not make much sense. Power
symbols don't translate to specific footprints in the layout. The symbol
does not represent a physical component.
* The pin number attribute should probably not be visible.
* The pin label and the pin number attributes are rotated by 180 degrees.
There is some evil magic in gschem that prevents them to render upside-down.
Still, there is a difference to upright orientation: The mark of the text
sits on the opposite side of the text. This makes it difficult to align the
text with other strings. My recommendation: Avoid 180° rotation in symbols.
* Your symbol is pretty large -- about three times the size of the power
symbols in the default library. Is this deliberate?
---)kaimartin(---
PS:
/your symbol file with comments by me--
# The version of gschem the symbol was created with
v 20091004 2
# three line statements
L 400 800 1000 800 3 0 0 0 -1 -1
L 500 700 900 700 3 0 0 0 -1 -1
L 600 600 800 600 3 0 0 0 -1 -1
# a pin statement. The attributes of the pin follow in curly brackets
P 700 1100 700 800 1 0 0
{
T 700 1100 5 10 0 0 0 0 1
pintype=pwr
# The pinlabel and the pinnumber are rotated by 180 degrees
T 505 500 5 10 0 1 180 6 1
pinlabel=PGND
T 605 1050 5 10 1 1 180 0 1
pinnumber=1
T 700 1100 5 10 0 0 0 0 1
pinseq=1
# The device attribute is inside the pin environment
T 400 400 5 10 1 1 0 0 1
device=PGND
T 600 1200 5 10 1 1 0 0 1
refdes=P?
}
\---
--
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: improved footprint for MSOP10
Stefan Salewski wrote: Please try to give more detailed error reports -- if that one is really wrong, we should remove it. The spacing of pads in the library footprint, checked visually and in the editor is very uneven. The centers of the pads are off the theoretical 0.5mm pitch by 0.1mm or so, which I find completely unacceptable. The footprint itself is from the 1-mil-time, not in 1/100-mil. Considering that the pad width is 0.3mm, the library version should really be replaced. Once agreement on my (modified) version is reached, I'll add the license. To yours: Do you really think that it is a good idea to have the text overlapping the pads by default position? At least *I* like it more than somewhere outside - I normally move the refdes anyway to enable tight packing of parts. If you want, you can put it at the top left corner. Well, iirc, this may be a bug with pcb, that wont handle a text position well in um-mode... The silk is close to the pads on the left and right side, at least distance is not symmetric on all four sides. I took great care to make the part symmetric, so it is. If you mean left and right margins are not equal to top and bottom, true. The reason is, that I kept the dimensions of the libary silk screen and made the pads longer for better hand soldering. Make the silk wider, if you like. Please note, it is a good idea to specify source of layout data and license for distribution. PCB footprints can have attributes for that. The source is probably a datasheet from Linear Technology. I realized that I left out a license after sending out... Hexadecimal flags may be OK, but textual ones seems to be preferred in these days. Is is really useful to have these thin soldermask areas between pads, or should we prefer a gang solder mask? With my manufacturer it is useful. I got the impression, that a gang solder mask will ruin your day. I do route on the inside of such a chip and wide solder mask gaps can lead to unnoticed shorts on the inside of legs. This is a question, I am not sure, but I think there is no real advantage for these stripes, but manufactures can have problems with it -- ok I think they remove it anyway. Piu-Printex doesn't remove the mask - if need be, they fab even smaller. But then again, they appear to be at the top end in Europe. 'multipcb' didn't complain either. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: improved footprint for MSOP10
Armin Faltl wrote: since the library version footprint MSOP10.fp seems to be very unprecise, I made my own, which is included below. How about an Armin_Faltl section in http://www.gedasymbols.org/ ? ---)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
gEDA-user: new footprint guidelines
Yes, the old library parts are pre-hires and the pads can be way off and should be fixed. Thanks! If we're hand-coding footprints, we could use 0.5mm instead of 1965 and preserve the *meaning* of the units. We lose some compatibility with older PCBs, but if the purpose is to update the current distribution that shouldn't be a problem. We should probably go with build-time generated footprint files, rather than continue to use the m4 runtime generation. That allows us to use more than just m4, too. Makefile rules for standard %.whatever to %.fp conversions... My general rules: Mask should be 3 mil away from copper, and slivers should be at least 6 mil wide. That means, if there's less than 12 mil between pads you go with a gang-opening. Silk should not overlap the *mask opening* and should be 3 mil away at least. 5 mil min silk lines. Origin and license should be stored in element attributes, not file comments, so they're copied into schematics. It would probably be a good idea to have more than one design for each footprint; one for reflow'd boards and one with longer pads for hand soldering. All QFN parts should have some visual aids to centering :-) On my last board, I added four diagonal lines on the silk layer to align each corner (like a big X), that worked out well. Refdes should be properly placed and sized but I'm not sure what's best. For example, on every single RESC1608N part I place I have to make the refdes smaller and move it off the pads. Getting size right is far more important than position; it's easy (and often needed anyway) to move things around in only-text mode. Exposed pads should have a proper solder paste pattern on them too. This usually means the one pad is made up of multiple pads, some with nopaste. I use one big nopaste pad and a small paste pad for each paste dot I want. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: new footprint guidelines
DJ Delorie wrote: [snip] All QFN parts should have some visual aids to centering :-) On my last board, I added four diagonal lines on the silk layer to align each corner (like a big X), that worked out well. During modifying library footprints, I found comments about placement lines, requesting additional non-fabrication layers like placement and outline. As there is currently no distinction on which layer an ElementLine[] would be, I suggest two mechanisms to achieve this: a) make the layername a text attribute in the flags. If no layer is named, silk is assumed. If there is no flag or layer of that name, again silk or autoinstantiate the layer. b) have an optional layer attribute behind the flags Option b) is more flexible I think. In that way, it would be quite nice to have some pure drawing layers besides a layer for part outlines to make center lines, rulers, dimensions and the like as in mechanical 2D cad. Actually I stumbled over this with placement of potentiometers, that have to be behind a hole drilled in the cover, LEDs etc. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: foreign graphics overlay
Dreaming about mechanical cad features in pcb and how one best works to mechanical constrains on a pcb, knowing the latest and greates pcb use OpenGL and transparency anyway, how about providing a plugin-mechanism, that allows to render DXF, SVG,..., bitmaps of common types and such on a non-functional translucent foreign layer? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
