I'm about to order a couple of PCBs from Olimex, this is the first time
ever I've done this, and just wondered what the common mistakes maybe?
Does anyone have a link to a website with helpful hints? I've looked
at the Olimex site which seems quite helpful just looking for any other
suggestions is Olimex a good idea for a beginner like me?
I've used Eagle and am not entirely sure what format is best to send
them too, they mention taking eagle files directly, those who use
Olimex, what format do you use?
The double sided boards, will they look like professionally mad boards,
ie with an insulating mask over the traces, and a silk screen of all
the stuff i've written in Ealge on the front?
Sorry if anyone feels these questions are answered in help or online
files, I just want to hear some personal feedback from anyone who have
used Olimex or similar to make their first PCB recently! I just don't
want to throw away money or look like an idiot....
> I'm about to order a couple of PCBs from Olimex, this is the first time
> ever I've done this, and just wondered what the common mistakes maybe?
> Does anyone have a link to a website with helpful hints? I've looked
> at the Olimex site which seems quite helpful just looking for any other
> suggestions is Olimex a good idea for a beginner like me?
Olimex has many hints on their site.
> I've used Eagle and am not entirely sure what format is best to send
> them too, they mention taking eagle files directly, those who use
> Olimex, what format do you use?
I used Eagle, after running Olimex's two Eagle macros. I wish I could
figure out how to configure the drills to Olimex's standards. In fact,
the ability to use Eagle files was one of the things that made Olimex
my choice.
> The double sided boards, will they look like professionally mad boards,
> ie with an insulating mask over the traces, and a silk screen of all
> the stuff i've written in Ealge on the front?
Ayup. My boards were great from Olimex. All the mistakes were mine.
> Sorry if anyone feels these questions are answered in help or online
> files, I just want to hear some personal feedback from anyone who have
> used Olimex or similar to make their first PCB recently! I just don't
> want to throw away money or look like an idiot....
Just remember to have some text off the board on *each* layer you want. I
just wrote the name of each layer. It looks funny, but it won't be in
your final boards and it helps them to keep the layers straight.
--
D. Jay Newman ! .....jayKILLspam@spam@sprucegrove.com ! Xander: Giles, don't make cave-slayer unhappy. http://enerd.ws/robots/ !
I'm not sure how, but change your Eagle drill list to suit the Olimex
drill list. Eagles drill list is different and Olimex will charge extra for
'non standard' sizes. Also make sure you have layer 20 (
dimentions ) enabled when you produce the files for olimex.
I attempted to produce a board using Eagle and Olimex. the basic
cost was FAR above base due to drill charges and other
'adjustments'.
The file format required is GERBER 274X
hth Mike W
--
On 24 Feb 04, at 18:09, Edward Cooper wrote:
> Hi
>
> I'm about to order a couple of PCBs from Olimex, this is the first
> time ever I've done this, and just wondered what the common mistakes
> maybe? Does anyone have a link to a website with helpful hints? I've
> looked at the Olimex site which seems quite helpful just looking for
> any other suggestions is Olimex a good idea for a beginner like me?
>
> I've used Eagle and am not entirely sure what format is best to send
> them too, they mention taking eagle files directly, those who use
> Olimex, what format do you use?
>
> The double sided boards, will they look like professionally mad
> boards, ie with an insulating mask over the traces, and a silk screen
> of all the stuff i've written in Ealge on the front?
>
> Sorry if anyone feels these questions are answered in help or online
> files, I just want to hear some personal feedback from anyone who have
> used Olimex or similar to make their first PCB recently! I just don't
> want to throw away money or look like an idiot....
>
> Thanks for any help.
>
> Ed
>
> --
> http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> email .....listservKILLspam.....mitvma.mit.edu with SET PICList DIGEST in the body
1. PCB production is usually a bit of a gamble, and I have got plenty of
boards back with mistakes in them even after years of practice. Double
checking everything is a very good idea. I have got to the point where I
budget half a day to carefully pick through a set of Gerber files before
sending them out. It takes ten minutes to make them and 4 hours to check
them. I also like to hand them off to another engineer or a technician to
check against the schematic, look for blunders, etc.
2. I have only worked by sending Gerber files to PCB houses, which is
rather tedious. If Olimex accepts Eagle raw data as you indicate (seems
like I remember they do) this will be easier on you.
3. Common mistakes with Gerber files:
leaving out a silkscreen layer
not adding a border to every layer for alignment (this is
unneccesary if sending Eagle files)
line wieght too small to print
Not checking the files carefully in a Gerber viewer before sending
Not putting your name, contact info, drawing and revision number
on every layer
Olimex should have guidelines on line weight. Some houses might say that
they cannot print test at less than 0.2mm line width, to pick a number out
of the air
4. Mistakes you might make in Eagle:
line wieghts or traces too thin
Stuff drawn on the wrong layer, for instance board outlines on the
copper layer
spacings too close
Component outlines inaccurate or interfering
Component outlines on the wrong side of the board
Not putting your name, contact info, drawing number and revision
number on the schematic and the board
Not putting a Revision number in the filename
Rev numbers not matching
If this is a production project I would budget at least three rounds of
PCB prototypes. As you gain experience, you should be able to reduce that
to one round and two in an occasional project that goes awry. If it is a
short run hobby project, expect to have some "change order wires' on the
board.
Revision numbers are important. Often the PCB house will catch a problem,
you will send them a rev, and they will go ahead and print the first set
you sent them because rev's are not clearly spelled out.
For any project, I would not push the line spacings and wifdths to less
than you absolutely need. Maybe Olimex can print 0.1mm lines at 0.1mm
spacings, but why push it? If .75 or 1mm traces will fit on your board
with 1mm spacings, give yourself some room. This is likely the case if it
is a thru-hole project.
Also, for very little extra money you can have some extra prototyping
boards. I usually add an array of 0.1" spaced thru-hole pads around the
board to fill it out to a handy size like 4" X 6".
On a later project you might consider panelizing your board to save money.
One 6"X6" board can cost less than 36 1"X1" boards. Don't bother with
that yet it adds complexity to an already tedious task.
-- Lawrence Lile
Senior Project Engineer
Toastmaster, Inc.
Division of Salton, Inc.
573-446-5661 voice
573-446-5676 fax
I'm about to order a couple of PCBs from Olimex, this is the first time
ever I've done this, and just wondered what the common mistakes maybe?
Does anyone have a link to a website with helpful hints? I've looked
at the Olimex site which seems quite helpful just looking for any other
suggestions is Olimex a good idea for a beginner like me?
I've used Eagle and am not entirely sure what format is best to send
them too, they mention taking eagle files directly, those who use
Olimex, what format do you use?
The double sided boards, will they look like professionally mad boards,
ie with an insulating mask over the traces, and a silk screen of all
the stuff i've written in Ealge on the front?
Sorry if anyone feels these questions are answered in help or online
files, I just want to hear some personal feedback from anyone who have
used Olimex or similar to make their first PCB recently! I just don't
want to throw away money or look like an idiot....
At 06:09 PM 2/24/2004 +0000, you wrote:
>Hi
>
>I'm about to order a couple of PCBs from Olimex, this is the first time
>ever I've done this, and just wondered what the common mistakes maybe?
>Does anyone have a link to a website with helpful hints? I've looked
>at the Olimex site which seems quite helpful just looking for any other
>suggestions is Olimex a good idea for a beginner like me?
Make sure that your silk screen text and outlines are at least 10 mil,
otherwise Olimex will fix this and charge you $5 extra.
Make sure that you use standard size drills from their mounted selection.
If you don't, there will be extra charges.
When you send them your design, they will run it through their tests, and
send you back what they object too.
>I've used Eagle and am not entirely sure what format is best to send
>them too, they mention taking eagle files directly, those who use
>Olimex, what format do you use?
>
>The double sided boards, will they look like professionally mad boards,
>ie with an insulating mask over the traces, and a silk screen of all
>the stuff i've written in Ealge on the front?
>Sorry if anyone feels these questions are answered in help or online
>files, I just want to hear some personal feedback from anyone who have
>used Olimex or similar to make their first PCB recently! I just don't
>want to throw away money or look like an idiot....
>
>Thanks for any help.
>
>Ed
>
>--
>http://www.piclist.com#nomail Going offline? Don't AutoReply us!
>email TakeThisOuTlistservEraseMEspam_OUTmitvma.mit.edu with SET PICList DIGEST in the body
Just a personal note on pcb's. I keep a procedure list, or check list, for
most of the things I do, generated from past errors. It can be a bit
tedious, but if you go through all the points before sending a job off,
problems will be minimal.
>Hi
>
>I'm about to order a couple of PCBs from Olimex, this is the first time
>ever I've done this, and just wondered what the common mistakes maybe?
>Does anyone have a link to a website with helpful hints? I've looked
>at the Olimex site which seems quite helpful just looking for any other
>suggestions is Olimex a good idea for a beginner like me?
>
>I've used Eagle and am not entirely sure what format is best to send
>them too, they mention taking eagle files directly, those who use
>Olimex, what format do you use?
>
>The double sided boards, will they look like professionally mad boards,
>ie with an insulating mask over the traces, and a silk screen of all
>the stuff i've written in Ealge on the front?
>
>Sorry if anyone feels these questions are answered in help or online
>files, I just want to hear some personal feedback from anyone who have
>used Olimex or similar to make their first PCB recently! I just don't
>want to throw away money or look like an idiot....
>
>Thanks for any help.
>
>Ed
>
>--
>http://www.piclist.com#nomail Going offline? Don't AutoReply us!
>email listservEraseME.....mitvma.mit.edu with SET PICList DIGEST in the body
>
Regards
Roland Jollivet
JeM Electric cc
PO Box 1460
Kloof
3640
Kwazulu Natal
South Africa
Tel: +27 31 7024412
Fax: +27 31 7011674 \o
Cell: +27 83 255 6017 l>
Email: EraseMEenquiriescaon.co.za < \
> Revision numbers are important. Often the PCB house will catch a problem,
> you will send them a rev, and they will go ahead and print the first set
> you sent them because rev's are not clearly spelled out.
Yes. The rev number and a quick copyright notice should be in the silkscreen
layer.
> On a later project you might consider panelizing your board to save money.
> One 6"X6" board can cost less than 36 1"X1" boards. Don't bother with
> that yet it adds complexity to an already tedious task.
It cost *much* less. However, Olimex will panelize and cut the boards
apart for free. I just sent them my Eagle file and a note to panelize
it. It probably would have been *much* more work to make two different
boards.
--
D. Jay Newman ! EraseMEjayspamspamBeGonesprucegrove.com ! Xander: Giles, don't make cave-slayer unhappy. http://enerd.ws/robots/ !
>From: Edward Cooper <edpgcSTOPspamspam_OUTDSL.PIPEX.COM>
>
>The double sided boards, will they look like professionally mad boards,
>ie with an insulating mask over the traces, and a silk screen of all
>the stuff i've written in Ealge on the front?
Well, they are professionally made boards :-) and, yes, they look like it.
Here's a couple of hints:
Use 10 mil minimum line width on the silk screen layer, including part
outlines, text, etc. This will probably mean changing some parts in the
libraries.
Use metric drill sizes that match their list.
And here's a couple of bloopers I did on my first board:
I drew a triangle (arrow) on the silkscreen layer with a zero-width border,
to make the angles sharper. This puts their plotting process into something
like an endless loop.
I neglected to put a border on the copper layer. They added one for me, but
unfortunately it shorted a couple of pads. Not hard to fix, but now I add
my own borders (like they say to do).
>
>Sorry if anyone feels these questions are answered in help or online
>files, I just want to hear some personal feedback from anyone who have
>used Olimex or similar to make their first PCB recently! I just don't
>want to throw away money or look like an idiot....
>
>Thanks for any help.
>
>Ed
>
>--
>http://www.piclist.com#nomail Going offline? Don't AutoReply us!
>email spamBeGonelistservSTOPspamEraseMEmitvma.mit.edu with SET PICList DIGEST in the body
D. Jay Newman says:
>I used Eagle, after running Olimex's two Eagle macros. I wish I could
>figure out how to configure the drills to Olimex's standards. In fact, the
>ability to use Eagle files was one of the things that made Olimex my choice.
My file "./scr/eagle.scr" contains this section:
BRD:
#Menu Add Change Copy Delete Display Grid Group Move Name Quit Rect \
# Route Script Show Signal Split Text Value Via Window ';' Wire Write
Edit;
grid mm;
SET Drill_Menu 0.7 0.9 1.0 1.1 1.3 1.5 2.1 3.3; grid mil;
change width 10;
change ratio 10;
I, in turn, put the date+time on each board, and use this as a revision
number. E.g., "make 50 of my Nov. 1, 2003 board."
>From: Mike W <@spam@mike@spam@spam_OUTCORN2.FREESERVE.CO.UK>
>
>I'm not sure how, but change your Eagle drill list to suit the Olimex
>drill list. Eagles drill list is different and Olimex will charge extra for
>'non standard' sizes.
Here's the script I use:
SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
Hazelwood Lyle says:
>Olimex offers lots of good suggestions on their site. the time spent =
>reading it is well spent. I sent them Eagle files directly. The board
>quality was excellent (by my own standard anyway) and included solder mask
>and silk screen.
When I got my first Olimex shipment, I carried the boards in my pocket for
a week and showed them to people in all sorts of settings. :-)
>I am a happy Olimex customer, and expect to do more with them in the =
>future. Just watch your drill sizes and understand that the silkscreen is
>a bit = low-res. For myself, I don't mind paying a few extra dollars to
>get extra drills = and/or getting their help fixing the silk layer.
The first board was so overwhelming. A major part of choosing Olimex was
that they were willing to take money and fix the small stuff, all without
berating me in public.
On my later boards, I made my own library parts from the original Eagle
parts. It seems that there should be a place on the PICList to post our
Olimex libraries. The mcintosh_to_olimex_030803.zip and
mcintosh_to_olimex_20031027.zip files in http://www.jump.net/~vima/PIC have
all been to Olimex, and returned boards that were pleasing. You can
recover the libraries from them if you wish, using exp-project-lbr.ulp. I
have a project named "local_library" and keep the modifications in there,
and the original CadSoft libraries in pristine condition.
>Somewhere on their site they specify exactly which layers are used from =
>Eagle for top, bottom, silk, and mask. by displaying only those layers,
>you should = be able to check your work before sending it off.
to the BRD: section of my Eagle.scr file. This is executed when a board is
loaded, so it display only the layers that Olimex will use, plus the
unrouted layer.
>On my later boards, I made my own library parts from the original Eagle
>parts. It seems that there should be a place on the PICList to post our
>Olimex libraries.
I even got the the point where I would create a blank library just for
a single project.. Each part would be copied in and edited to suit the
board maker I plan to send it off to. This makes creating consistent
parts much easier to organize. It also prevents the need to edit the
oriiginal libraries just to use the recommended drills.
> Here's the script I use:
> SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
>
> Set the grid to mm before you run it.
>
> Colin
Cheers everyone for your help, some invaluable advice there!
Colin- Will this change the holes that are already there? If not is
there a way I can get Eagle to just round up the drill sizes to the
nearest one in that selection? I've just mainly used parts that are in
Eagles default libraries which have imperial size holes I think, would
prefer to switch everything over to mm because they are so much easier!
At 06:09 PM 2/24/2004 +0000, you wrote:
>Hi
>
>I'm about to order a couple of PCBs from Olimex, this is the first time
>ever I've done this, and just wondered what the common mistakes maybe?
General rules, not specific to this company or layout program:
Run DRC and check annular ring size with final drill sizes. Watch that
silk screen markings (which always seem unimportant) don't wind up on
SMT pads. Double check all hole sizes. You do NOT want them too small,
and too big is almost as bad. Check power pins to make sure there isn't
an isolated net that didn't get connected; it's often a good idea to go
through the netlist and just look at everything there. Make sure you
don't do anything really stupid like flipping a part or getting the
wrong footprint by printing out the PCB 1:1 and setting parts on
top of it. Especially double check footprints that you created for
wrong pin numbers relative to their schematic and physical layout.
>From: Edward Cooper <RemoveMEedpgcEraseMEspam_OUTDSL.PIPEX.COM>
>
>Cheers everyone for your help, some invaluable advice there!
>
>Colin- Will this change the holes that are already there? If not is
>there a way I can get Eagle to just round up the drill sizes to the
>nearest one in that selection?
There might be a ULP that does this, but I'm not so sure it's a good idea.
There's bound to be some judgment calls.
Note that there's no 0.8 mm drill, so 0.031 in. holes for a 5 mm LED, for
example, would round down to 0.7 mm, which would be too small. Now, 0.032
in. holes woiuld round up to 0.9 mm which would be OK, except that, if the
pad diameter is fixed, you could end up with an annular ring that is too
narrow; and if the pad width is set to auto you could end up with a pad
that is too wide.
Best to just get in there and set the hole and diameter to what you want;
you can group the pads, after all . Some folks have suggested letting the
board house worry about it but I'm not at all comfortable with that.
Colin, once you change to mm rather than Imperial you loose the
board consistancy.. unless I'm missing something here..
Eagle is a bastard when trying to locate or position anything on a
grid that its not set for.. mm component on imp grid and vice
versa.. do I explain myself adequatley?.
Excellent software, but limitations AFIK
...
--
On 24 Feb 04, at 13:09, Colin Constant wrote:
> >From: Mike W <EraseMEmike@spam@CORN2.FREESERVE.CO.UK>
> >
> >I'm not sure how, but change your Eagle drill list to suit the Olimex
> >drill list. Eagles drill list is different and Olimex will charge
> >extra for 'non standard' sizes.
>
> Here's the script I use:
> SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
>
> Set the grid to mm before you run it.
>
> Colin
>
> _________________________________________________________________ The
> new MSN 8: advanced junk mail protection and 2 months FREE*
> join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjo
> in.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca
>
> --
> http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> email @spam@listservspam_OUT.....mitvma.mit.edu with SET PICList DIGEST in the body
You don't have to change to mm - Olimex will pick the closest drill. If you
look on their web site, you will see there drill list in metric and US
measurments.
>Colin, once you change to mm rather than Imperial you loose the
>board consistancy.. unless I'm missing something here..
>Eagle is a bastard when trying to locate or position anything on a
>grid that its not set for.. mm component on imp grid and vice
>versa.. do I explain myself adequatley?.
>Excellent software, but limitations AFIK
>...
>--
>On 24 Feb 04, at 13:09, Colin Constant wrote:
>
> > >From: Mike W <mikespamBeGoneCORN2.FREESERVE.CO.UK>
> > >
> > >I'm not sure how, but change your Eagle drill list to suit the Olimex
> > >drill list. Eagles drill list is different and Olimex will charge
> > >extra for 'non standard' sizes.
> >
> > Here's the script I use:
> > SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
> >
> > Set the grid to mm before you run it.
> >
> > Colin
> >
> > _________________________________________________________________ The
> > new MSN 8: advanced junk mail protection and 2 months FREE*
> > join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjo
> > in.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca
> >
> > --
> > http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> > email RemoveMElistserv@spam@spamBeGonemitvma.mit.edu with SET PICList DIGEST in the body
>
>--
>http://www.piclist.com#nomail Going offline? Don't AutoReply us!
>email .....listserv@spam@EraseMEmitvma.mit.edu with SET PICList DIGEST in the body
> You don't have to change to mm - Olimex will pick the closest drill. If you
> look on their web site, you will see there drill list in metric and US
> measurments.
That's what's implied, but they charged me $1.20 for a non-metric drill.
Not that I'm complaining, mind you. My next board goes to Olimex also.
--
D. Jay Newman ! .....jaySTOPspam@spam@sprucegrove.com ! Xander: Giles, don't make cave-slayer unhappy. http://enerd.ws/robots/ !
The one blooper I made with Olimex (at least I think it's my blooper) is that many of the hole sizes for the parts ended up being too small. I use the default sizes for standard parts like DIP16 etc.
I had to re-drill many of the holes. It was only 14 boards with about 50 holes or so that needed to be re-drilled per board.
But when you add that up it's 700 holes to drill by hand.
Next time I send a board out to them I will measure every pin with the calipers a re-check all my holes!
Previously I used ExpressPCB and their software and did not have any of these problems.
On the positive side... I got 14 1-sided boards (about 2" x 5" for less than 100$ U.S.)
Which came up to be quite a bit less than anywhere else I looked at.
>Sorry if anyone feels these questions are answered in help or online
>files, I just want to hear some personal feedback from anyone who have
>used Olimex or similar to make their first PCB recently! I just don't
>want to throw away money or look like an idiot....
> -----Original Message-----
> From: pic microcontroller discussion list
> [spamBeGonePICLISTKILLspam@spam@MITVMA.MIT.EDU]On Behalf Of Gustaf J. Barkstrom
> Sent: Tuesday, February 24, 2004 9:56 PM
> To: PICLISTspam_OUT@spam@MITVMA.MIT.EDU
> Subject: Re: ] My first PCB production
>
>
> > I'm about to order a couple of PCBs from Olimex, this is the first time
> > ever I've done this, and just wondered what the common mistakes maybe?
>
> A couple of boards, as in two? I have been following this thread, but as
> I've gotten
> back into electronics in the last couple months, I've rounded up items
> to make my own PCBs. Is the project sufficiently complext that you can't
> make the boards yourself? If you are only making a couple of boards, I
> would
> invest in some small supplies to do it yourself. Of course, there are two
> factors that have allowed me to not need PCB services yet: 1) I have lots
> of extra time, no wife, no children, etc.; 2) I don't have any really
> complex
> board designs (yet). And of course, my boards are only 1 or 2 sided, no
> silkscreen,
> and so forth.
>
> Gustaf
>
> <snip>
> >
> > Ed
> >
> > --
> > http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> > email spamBeGonelistserv@spam@mitvma.mit.edu with SET PICList DIGEST in the body
> >
>
> --
> http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> email RemoveMElistservEraseMEKILLspammitvma.mit.edu with SET PICList DIGEST in the body
>
Just FYI - I have used Olimex for protos and a small production run.
Proto's only from now on.
I just had a production run from E-TEK Net (http://e-teknet.com/) in
Arizona, Phoenix area. A little more $$ than Olimex, but still very cost
competitive. Excellent quality and no restrictions on drill sizes, etc. I
think they go down to 6 mil traces / gaps. Dan Ditto is a good contact
point. I have no relationship with these guys, just like their quality,
pricing and service
> Actually, there is more Olimex-like producers.
> I gathered about fifteen links I think at http://www.radier.ca/pic/list.php
> And there is more - mostly europeans at http://www.cadsoftusa.com
> under Boardhouses.
>
> Dmitriy.
>
>
> {Original Message removed}
Another thumbs up for E-Teknet.
Their shipping is VERY fast, for me the pricing was better than Olimex for
100 pc runs, and they included electrical testing no charge.
10 business days from the time I email my gerbers to the time I have PC
boards in my hands.
Dave
> I just had a production run from E-TEK Net (http://e-teknet.com/) in
> Arizona, Phoenix area. A little more $$ than Olimex, but still very cost
On Tuesday, Feb 24, 2004, at 13:20 US/Pacific, Edward Cooper wrote:
>> Here's the script I use:
>> SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
>
> Colin- Will this change the holes that are already there?
No. I'm also pretty sure it doesn't change the hole sizes in
any parts you get from libraries.
> If not is there a way I can get Eagle to just round up the
> drill sizes to the nearest one in that selection?
Eagle will do all sorts of things like that when you export
to gerber-style formats, but I haven't found a good way of
modifying things in the Eagle-format files themselves.
(other than modifying all the libraries.) There's a similar
problem with the silkscreen layer; there are nice ULPs to
regenerate a silkscreen layer with adjusted line widths,
but they generate a NEW silkscreen layer rather than modifying
the existing layers...
It ought to be possible to export all the parts in a given
board as a new library, and then adjust the hole sizes and
line widths in that library, and then re-aim/update the board
to use the adjusted library, but the last time i tried to do
this I ran into assorted problems and didn't pursue it.
(This would be a ULP. Only one person has to write it, and
then anyone can use it.) IIRC, you could export all the parts
to a single library file, but the board would still point at
"part@file" type designators (multiple files for the board.)
You could output a directory hierarchy of modified libraries
and point the board at the new directory, but I thought that
was a bit messy... Sigh. (I guess it's a pretty flat
hierarchy; might not be THAT bad...)
Olimex will combine your designs and separate the boards, all for free.
Are there any boardhouses in the list that beat their price for let's
say 20 different designs, 1 ex each? If the designs fit together on a
16x10 cm Olimex will do this for $26 (DS, +extra holes, +shipping).
Have tried this link twice and got an error message both time.
CR
>
>
> > I just had a production run from E-TEK Net (http://e-teknet.com/) in
> > Arizona, Phoenix area. A little more $$ than Olimex, but still very
cost
>
But that seems to be only if you win the contest for that month *and*
use a PIC in your design (given this list, that isn't improbable).
--
D. Jay Newman ! spam_OUTjayKILLspamsprucegrove.com ! Xander: Giles, don't make cave-slayer unhappy. http://enerd.ws/robots/ !
Just looked at the site. Interesting.
Are there limits; age/status/..
And geographical, worldwide?
Regards
Roland
At 09:37 AM 25/02/04 -0800, you wrote:
>And Olimex will give you a free PCB panel if you publish your design:
>http://www.piclist.com/techref/piclist/pcbcontest.htm
>
>
>---
>James.
>
>
>{Original Message removed}
Talking of Olimex, I noticed they now have an ICD2 clone complete with USB
interface for $89.95 Anyone bought this?
Regards
Mike
=======================================================================
This e-mail is intended for the person it is addressed to only. The
information contained in it may be confidential and/or protected by
law. If you are not the intended recipient of this message, you must
not make any use of this information, or copy or show it to any
person. Please contact us immediately to tell us that you have
received this e-mail, and return the original to us. Any use,
forwarding, printing or copying of this message is strictly prohibited.
No part of this message can be considered a request for goods or
services.
=======================================================================
Any questions about Bookham's E-Mail service should be directed to RemoveMEpostmasterspamBeGoneRemoveMEbookham.com.
You can change back to imperial after you fix the holes. But you're probably
going to execute the script in the library anyway, so it won't affect the
board.
>
>Colin, once you change to mm rather than Imperial you loose the
>board consistancy.. unless I'm missing something here..
>Eagle is a bastard when trying to locate or position anything on a
>grid that its not set for.. mm component on imp grid and vice
>versa.. do I explain myself adequatley?.
>Excellent software, but limitations AFIK
>...
>--
>On 24 Feb 04, at 13:09, Colin Constant wrote:
>
> > >From: Mike W <@spam@mikeSTOPspam@spam@CORN2.FREESERVE.CO.UK>
> > >
> > >I'm not sure how, but change your Eagle drill list to suit the Olimex
> > >drill list. Eagles drill list is different and Olimex will charge
> > >extra for 'non standard' sizes.
> >
> > Here's the script I use:
> > SET DRILL_MENU .7 .9 1 1.1 1.3 1.5 2.1 3.3;
> >
> > Set the grid to mm before you run it.
> >
> > Colin
> >
> > _________________________________________________________________ The
> > new MSN 8: advanced junk mail protection and 2 months FREE*
> > join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjo
> > in.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca
> >
> > --
> > http://www.piclist.com#nomail Going offline? Don't AutoReply us!
> > email listservspamBeGonespamBeGonemitvma.mit.edu with SET PICList DIGEST in the body
>
>--
>http://www.piclist.com#nomail Going offline? Don't AutoReply us!
>email spamBeGonelistservmitvma.mit.edu with SET PICList DIGEST in the body
On Thursday, Feb 26, 2004, at 09:06 US/Pacific, Colin Constant wrote:
>> Colin, once you change to mm rather than Imperial you loose the
>> board consistancy.. unless I'm missing something here..
>> Eagle is a bastard when trying to locate or position anything on a
>> grid that its not set for...
You can change inches to mm without problems, just let Eagle
recompute the size. Your default .05 inch grid becomes a
1.27 mm grid, and none of the grid lines actually move anywhere.
BillW
-- http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads
What is the correct topic for this discussion?
I have adjusted it to [EE]
I have never heard of ammonium perchlorate. I have heard of and use ammonium
persulfate and sodium persulfate with excellent results. It is very safe. Its
fumes are no where near as bad as ferric chloride and the spent solution is
almost neutral and it does not stain and corrode everything it comes near and
is easy to dispose of.
Rick
> Oyvind,
>
> It is ammonium perchlorate. Its fumes are nastier than ferric chloride
> in my opinion. But, it does allow one to see the etching process through
> the liquid, unlike ferric chloride. As always; ventilation, ventilation,
> ventilation. Oh, and safety googles of course. Don't take your vision for
> granted. :)
>
> Gustaf
>
> >
> > What is the "Magic White powder" exactly?
> >
> > Oyvind
>
> --
Anthony Toft wrote:
> Yes but you can electro-plate the copper from the spent echant, changing it
> back to FeCl, just use some nails for the electrodes. No need to throw any
> away, just keep reusing it.
When I look at the specs from board houses, they all say similar things:
xx oz copper laminated on board...
xx more copper plated on after etching...
xx solder reflow after plating ...
So, how can I as a homebrewer "reuse" all this extra copper and plate it back
on my board where I want it instead of on my nails:-)
> I would not consider it immoral or illegal to dump small quantities
> of chemicals down the drain once I was told by local authorities
> that it's acceptable to do so
Living in a marine environment I wouldn't dump soluble copper down
the drain even if some desk-jockey at the local council said it was OK
At the very least I'd make it into a solid (eg drop the copper out with
sodium carbonate) as you suggest, and send that sludge to the tip.
Still not the ideal, and a tip shouldn't really be taken for granted and
expected to be an environmental basket-case. For the same reasons
I wouldn't send old lead or NiCd batteries out in the general rubbish
>When I look at the specs from board houses, they all say similar things:
>
> xx oz copper laminated on board...
> xx more copper plated on after etching...
> xx solder reflow after plating ...
>
>So, how can I as a homebrewer "reuse" all this extra copper and plate
>it back on my board where I want it instead of on my nails:-)
I doubt it is plated on after etching.
My understanding is that the normal way to do things is to put on a resist
over the areas that are going to be etched away.
Then drill the holes (or these first two steps may be reversed).
The board is then put in a solution to chemically deposit a base for the
copper down the drilled holes.
The board is then electroplated with copper to get the plated through holes
to have copper to the desired thickness. An inherent part of this process is
that the copper lands also receive a plating of copper, increasing their
thickness.
The tin electroplate is then plated on.
The resist is then removed.
The board is then etched to the desired pattern, using the tin electroplate
as a resist for the etchant.
This is the way I was told it is done. I have never actually tried it. It
may be that processes have changed since then, as it was a while ago that it
was described to me.
-- http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads
> Regarding standard Ferrous Copper Chloride solution (which
> may not be what type of chemcials you are referring to), the
> water company actually adds this to the drinking water anyways
To precipitate things like copper ?
I'm pretty sure Fe isn't anywhere near as toxic as Cu. Not that I'd
drink out of a rusty bucket if I didn't have to
Many things are bio-active in minute doses. eg hormones, LSD,
radiation sources. My litre of spent FeCl might not be much in the
greater scheme of things but I'd still try to be good. Unfortunately
we've moved on from sitting around in caves not polluting and there's
some responsibility that comes with that
(I hate the scourge of excess packaging too BTW)
-- http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads
On Tuesday, Mar 2, 2004, at 01:50 US/Pacific, Alan B. Pearce wrote:
>>
>> So, how can I as a homebrewer "reuse" all this extra copper and plate
>> it back on my board where I want it instead of on my nails:-)
>
> I doubt it is plated on after etching.
>
> My understanding is that the normal way to do things...
There's a good (last time I looked) description of the "normal" PCB
process at http://www.thinktink.com, and on a couple of the PCB shop websites.
It tends to go something like this:
1) drill.
2) Plate through holes. (You want to have solid copper on both sides
for this step, for nice solid electrical conductivity from the
connection point to each of the holes...)
3) apply resist, expose via photo of some sort.
4) Strip resist from areas where there WILL be tracks. "develop"
5) tin/lead plate (onto the spots that will be tracks.)
6) strip resist from rest of board.
7) nasty but generally replenishable etchants etch away copper
except where it is tin/lead plated.
Somehow getting the copper from the etch part of the cycle back to
the plating part of the cycle is an interesting idea. I don't know
whether it's done or not. In any case, you'll still wind up with
extra copper, since you etch most of it off again. if you have a
use for copper, there are assorted places ("Industrial reuse") that
will sell you copper sulfate in solution for pretty cheap, or free:
<apps01.metrokc.gov/govlink/hazwaste/business/imex/
getlistings.cfm?cat=3&aw=A>
mitvma.mit.edu with SET PICList DIGEST in the body
