Post by thread:[EE:] My first PCB production

Exact match. Not showing close matches.
PICList Thread
'[EE:] My first PCB production'
2004\02\24@130934 by Edward Cooper

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 spam_OUTlistservTakeThisOuTmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@131552 by D. Jay Newman

> 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/ ! -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email listservKILLspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@132555 by Mike W

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: {Quote hidden}> 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 -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email EraseMElistservspam_OUTTakeThisOuTmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@133353 by llile

Edward, 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 Edward Cooper <edpgcspam_OUTDSL.PIPEX.COM> Sent by: pic microcontroller discussion list <@spam@PICLISTKILLspamMITVMA.MIT.EDU> 02/24/2004 12:09 PM Please respond to pic microcontroller discussion list To: KILLspamPICLISTKILLspamMITVMA.MIT.EDU cc: Subject: [EE:] My first PCB production 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 RemoveMElistservTakeThisOuTmitvma.mit.edu with SET PICList DIGEST in the body -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spamBeGonelistservspamBeGonemitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@133806 by Larry Bradley

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? Yes indeed. {Quote hidden}>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 Larry Bradley Orleans (Ottawa), Ontario, CANADA -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservTakeThisOuTmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@134639 by Roland

Hi 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. At 06:09 PM 24/02/04 +0000, you wrote: {Quote hidden}>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 < \ -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservEraseMEEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@135302 by D. Jay Newman

> At 06:09 PM 2/24/2004 +0000, you wrote: > Make sure that you use standard size drills from their mounted selection. > If you don't, there will be extra charges. Yes, but the charges are fairly minimal. Frankly the charges are less than my time is worth to change the part libraries I use to fit their format. And as somebody else suggested, next time I will use faster shipping. -- D. Jay Newman ! RemoveMEjayspam_OUTKILLspamsprucegrove.com ! Xander: Giles, don't make cave-slayer unhappy. http://enerd.ws/robots/ ! -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservTakeThisOuTspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@135718 by D. Jay Newman

> 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/ ! -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservKILLspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@140547 by Colin Constant

>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). Colin {Quote hidden}> >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 _________________________________________________________________ Help STOP SPAM with the new MSN 8 and get 2 months FREE* http://join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjoin.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email KILLspamlistservspamBeGonemitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@150106 by Intosh, Ph.D.

-----BEGIN PGP SIGNED MESSAGE----- Hash: SHA1 source= http://www.piclist.com/piclist/2004/02/24/131552a.txt? 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." - --- Aubrey McIntosh http://www.piclist.com/member/AM-vima-Y84 PIC/PICList FAQ: http://www.piclist.com -----BEGIN PGP SIGNATURE----- Version: PGPfreeware 7.0.3 for non-commercial use <http://www.pgp.com> iQA/AwUBQDus5QKlSw8yssF7EQIfBACgg94n8gtOQRRfqMM+vYax8Vo0t9gAn3h3 C9UltfYfQPPsTgV6E5Ga9EeU =wOVI -----END PGP SIGNATURE----- -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email EraseMElistservEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@151141 by Colin Constant

>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; Set the grid to mm before you run it. Colin _________________________________________________________________ The new MSN 8: advanced junk mail protection and 2 months FREE* http://join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjoin.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spamBeGonelistservKILLspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@152808 by Intosh, Ph.D.

-----BEGIN PGP SIGNED MESSAGE----- Hash: SHA1 source= http://www.piclist.com/piclist/2004/02/24/132805a.txt? 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. Just after my last post, I also added the line: display none top bottom 17 18 20 21 25 -23 -27 -51 unrouted; 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. - --- Aubrey McIntosh http://www.piclist.com/member/AM-vima-Y84 PIC/PICList FAQ: http://www.piclist.com -----BEGIN PGP SIGNATURE----- Version: PGPfreeware 7.0.3 for non-commercial use <http://www.pgp.com> iQA/AwUBQDuzWgKlSw8yssF7EQKpXQCgoJMQGS0L6gvIG8OPCy8jkR8b+Q8An3lI 1akFGC+rzoqD1Xzrza48kVuG =xOK5 -----END PGP SIGNATURE----- -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email .....listservspam_OUTmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@153428 by Hazelwood Lyle

>From: Aubrey McIntosh, Ph.D. [TakeThisOuTAubrey.McIntosh.....TakeThisOuTALUMNI.UTEXAS.NET] >Subject: Re: [EE:] My first PCB production >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. Lyle -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email TakeThisOuTlistservKILLspamspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@155853 by Colin Constant

>From: "Aubrey McIntosh, Ph.D." <.....Aubrey.McIntoshRemoveMEALUMNI.UTEXAS.NET> >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. :-) You too?? It's amazing how polite people can be, isn't it? I response to the inevitable "What does it do?" I just say "Well, nothing, but it sure looks pretty, doesn't it?" Colin _________________________________________________________________ Add photos to your e-mail with MSN 8. Get 2 months FREE*. http://join.msn.com/?page=features/photos&pgmarket=en-ca&RU=http%3a%2f%2fjoin.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservspamBeGonemitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@162137 by Edward Cooper

> 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! Thanks Ed -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spamBeGonelistserv@spam@spam_OUTmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@162142 by Spehro Pefhany

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. Best regards, Spehro Pefhany --"it's the network..." "The Journey is the reward" TakeThisOuTspeffspaminterlog.com Info for manufacturers: http://www.trexon.com Embedded software/hardware/analog Info for designers: http://www.speff.com -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email listservEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@180558 by Colin Constant

>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 _________________________________________________________________ Add photos to your messages with MSN 8. Get 2 months FREE*. http://join.msn.com/?page=dept/features&pgmarket=en-ca&RU=http%3a%2f%2fjoin.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email @spam@listservRemoveMEEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@191809 by Mike W

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: {Quote hidden}> >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 -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spamBeGonelistservEraseMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@201341 by Larry Bradley

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. At 12:12 AM 2/25/2004 +0000, you wrote: {Quote hidden}>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 Larry Bradley Orleans (Ottawa), Ontario, CANADA -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email .....listservRemoveMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@205942 by D. Jay Newman

> 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/ ! -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email listservEraseME@spam@mitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@213138 by Michael J. Pawlowsky

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.... -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email RemoveMElistservspamBeGonemitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@220125 by Gustaf J. Barkstrom

Err, MS Outlook modified my subject line... back on thread now... sorry. {Quote hidden}> -----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 > -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spamBeGonelistservspam_OUTRemoveMEmitvma.mit.edu with SET PICList DIGEST in the body

2004\02\24@230636 by Dmitriy Fitisov

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}

2004\02\24@235441 by Chuck Busch

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 Chuck ----- Original Message ----- From: "Dmitriy Fitisov" <.....dmitriyRemoveMERADIER.CA> To: <PICLIST@spam@MITVMA.MIT.EDU> Sent: Tuesday, February 24, 2004 8:04 PM Subject: Re: [EE:] My first PCB production > 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}

2004\02\24@235854 by David Schmidt

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 -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email EraseMElistservRemoveMESTOPspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\25@023927 by Luis Moreira

Hi guys does any one knows of a prototype PCB manufacturer like Olimex in the UK regards Luis {Original Message removed}

2004\02\25@030040 by William Chops Westfield

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...) BillW -- http://www.piclist.com hint: To leave the PICList RemoveMEpiclist-unsubscribe-requestKILLspamTakeThisOuTmitvma.mit.edu

2004\02\25@042326 by Wouter van Ooijen

> 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. 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). Wouter van Ooijen -- ------------------------------------------- Van Ooijen Technische Informatica: http://www.voti.nl consultancy, development, PICmicro products -- http://www.piclist.com hint: To leave the PICList spamBeGonepiclist-unsubscribe-request@spam@mitvma.mit.edu

2004\02\25@051057 by Brian Clewer

Luis wrote: > > Hi guys > does any one knows of a prototype PCB manufacturer like Olimex in the UK > regards > Luis They are not in the UK, but Ireland. They are usually very good (and cheap). Will ship to the UK in 2-3 days. http://www.pcb-pool.com Brian. -- http://www.piclist.com hint: To leave the PICList RemoveMEpiclist-unsubscribe-requestspam_OUTmitvma.mit.edu

2004\02\25@085314 by Charles Rogers

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 > -- http://www.piclist.com hint: To leave the PICList piclist-unsubscribe-requestspammitvma.mit.edu

2004\02\25@100508 by David Schmidt

www.e-teknet.com > Have tried this link twice and got an error message both time. -- http://www.piclist.com hint: To leave the PICList spam_OUTpiclist-unsubscribe-requestspam_OUTspam_OUTmitvma.mit.edu

2004\02\25@105056 by Chuck Busch

Just did it again...worked fine. http://e-teknet.com/ ----- Original Message ----- From: "Charles Rogers" <crogersspam_OUTGBRONLINE.COM> To: <RemoveMEPICLISTKILLspam@spam@MITVMA.MIT.EDU> Sent: Wednesday, February 25, 2004 5:52 AM Subject: Re: [EE:] My first PCB production {Quote hidden}> 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 > > > > -- > http://www.piclist.com hint: To leave the PICList > piclist-unsubscribe-requestspamBeGone.....mitvma.mit.edu -- http://www.piclist.com hint: To leave the PICList KILLspampiclist-unsubscribe-request.....mitvma.mit.edu

2004\02\25@124030 by James Newton, Host

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}

2004\02\25@125730 by D. Jay Newman

> And Olimex will give you a free PCB panel if you publish your design: > http://www.piclist.com/techref/piclist/pcbcontest.htm 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/ ! -- http://www.piclist.com hint: To leave the PICList RemoveMEpiclist-unsubscribe-requestRemoveMEEraseMEmitvma.mit.edu

2004\02\25@131803 by Roland

Hi James 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}

2004\02\25@133511 by hael Rigby-Jones

>-----Original Message----- >From: James Newton, Host [KILLspamjamesnewtonspamBeGonePICLIST.COM] >Sent: 25 February 2004 17:38 >To: PICLISTspamMITVMA.MIT.EDU >Subject: Re: [EE:] My first PCB production > > >And Olimex will give you a free PCB panel if you publish your >design: http://www.piclist.com/techref/piclist/pcbcontest.htm > 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. -- http://www.piclist.com hint: To leave the PICList KILLspampiclist-unsubscribe-requestspamBeGonemitvma.mit.edu

2004\02\26@120907 by Colin Constant

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 {Quote hidden}> >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 _________________________________________________________________ Help STOP SPAM with the new MSN 8 and get 2 months FREE* http://join.msn.com/?page=dept/bcomm&pgmarket=en-ca&RU=http%3a%2f%2fjoin.msn.com%2f%3fpage%3dmisc%2fspecialoffers%26pgmarket%3den-ca -- http://www.piclist.com hint: PICList Posts must start with ONE topic: [PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads

2004\02\26@143337 by William Chops Westfield

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

2004\02\29@104324 by Rick C.

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 "Gustaf J. Barkstrom" wrote: {Quote hidden}> 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 > > -- -- http://www.piclist.com#nomail Going offline? Don't AutoReply us! email spam_OUTlistservSTOPspammitvma.mit.edu with SET PICList DIGEST in the body

2004\02\29@105323 by Gustaf J. Barkstrom

Ack! My mistake. It's ammonium persulfate. You are correct, it's safer and more neutral. Also supposed to be much faster than ferric chloride. Going back under my rock now. Gustaf > {Original Message removed}

'[EE:] My first PCB production'
2004\03\01@142959 by John Plocher

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:-) -John -- http://www.piclist.com hint: To leave the PICList RemoveMEpiclist-unsubscribe-requestspammitvma.mit.edu

2004\03\01@164027 by Jinx

> 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 -- http://www.piclist.com hint: To leave the PICList TakeThisOuTpiclist-unsubscribe-requestspamRemoveMEmitvma.mit.edu

2004\03\02@045121 by Alan B. Pearce

>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

2004\03\02@164550 by Jinx

> 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

2004\03\03@013433 by William Chops Westfield

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> BillW -- http://www.piclist.com hint: The list server can filter out subtopics (like ads or off topics) for you. See http://www.piclist.com/#topics

More... (looser matching)
- Last day of these posts
- In 2004 , 2005 only
- Today
- New search...