Re: [PEDA] irregular shaped holes ??
Robison Michael R CNIN wrote: thanks for the suggestion about putting some text inside the cutout area. one thing i tend to forget is that people do actually look at the gerbers. i get in this mode where i think all they do is blindly submit them to a machine and a pcb comes out the other end. i'll make a readme file too. miker Miker - here is a sample of the readme file I send out with a PCB order: From: Peter Bennett TRIUMF 4004 Wesbrook Mall Vancouver, B.C. V6T 2A3 Phone: 222-7456 FAX: 222-7307 email: [EMAIL PROTECTED] TRIUMF P.O. # TR 137029 Job:0946 Scanning ADC PC Board P-13151 The following files are required for this job: p13151.GTL Component side copper photoplot file p13151.GBL Solder side copper photoplot file p13151.GTO Component layout silkscreen p13151.GBS Bottom Solder Mask p13151.GTS Top Solder Mask p13151.TXT Drill file readme.txtThis file Note: the Gerber files include embedded aperture data. Drill Information Tool Hole Size Hole Count Plated Tool Travel --- T125mil (0.635mm) 159 75.20 Inch (1909.99 mm) T235mil (0.889mm) 647 124.45 Inch (3161.07 mm) T347mil (1.1938mm) 74 24.86 Inch (631.56 mm) T455mil (1.397mm) 15 16.77 Inch (426.00 mm) T570mil (1.778mm) 23.59 Inch (91.19 mm) T6125mil (3.175mm) 10 27.48 Inch (697.97 mm) T7141mil (3.5814mm)311.16 Inch (283.47 mm) --- Totals 910 283.51 Inch (7201.24 mm) The board is 7.20 x 11.6, +/- .010, double-side, .0625 nominal thickness, FR-4 material 1 oz or greater copper Standard through-hole plating, standard tin-lead plating on exposed copper. Standard gold plating on edge connector Solder mask both sides (different masks) Component Ident silkscreen on component side (ident not required on bottom) Trim boards to outline on component side artwork Please make at least 3 boards. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] irregular shaped holes ??
hello, i've never had to place an irregular shaped hole in a board before, and i can't figure out how to do it. i looked up drill, hole, and irregular in the help and had no luck. its essentially an elongated circle. i kinda figure that it involves perhaps placing some lines and arcs on a specific mechanical layer, but thats as far as i can get. all the holes i have placed so far have been done with the pad tool. i notice that you can adjust the shape of the solder ring using this tool, but not the hole shape itself. thank you, miker * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] irregular shaped holes ??
Robison Michael R CNIN wrote: thanks peter, recently we acquired some gerbers for a board that had a hole in it that was used as a handle. i tweeked some of the silkscreening and sent it off to advanced circuits and they produced the board with no problem. i did call them and ask if they could do irregular holes (not pads) first. so there is evidently some sort of standard for denoting these sort of holes. unfortunately, its difficult for me to reverse engineer the former card's gerbers to see what sort of actions i need to take in protel to produce it. hmm... i've got an idea now. i went to tools/preferences/display/ and selected single layer mode and went thru the various layers and the mechanical4 is the only layer which displayed the army- green board outline. i'm gonna venture a (dangerous) guess that if i put the hole outline on this layer that it would be noted as a hole. any general consent on that? If you include Mech4 on the gerbers for the copper layers that should work. For large cutouts like that, I would also place text in the area to be removed saying Cutout 1 x 4 to indicate the area to be removed, and its approximate size, as well as mentioning the cutout in the readme file. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] irregular shaped holes ??
On 04:39 PM 18/07/2001 -0500, Robison Michael R CNIN said: thanks peter, ..snip.. hmm... i've got an idea now. i went to tools/preferences/display/ and selected single layer mode and went thru the various layers and the mechanical4 is the only layer which displayed the army- green board outline. i'm gonna venture a (dangerous) guess that if i put the hole outline on this layer that it would be noted as a hole. any general consent on that? thanks again, miker If you label it as a slot and add appropriate info in the manufacturing notes then this should work fine. It is basically what I do. I would typically dimension and add start and end coords of the slot (on a different mech layer). The PCB maker has to interpret what the details on the Mech layers mean. If you add appropriate strings and coords and dimension you can easily make it clear what is required. Basically there is no method, in Protel at least, to convey any sort of slot. You basically use the non-electrical (usually mech or drill drw layers) to specify the slot and then add info in manufacturing details. If it is complex you then ring the PCB maker to make sure the understand exactly. I have done one board with a mix of complex outline routes, large routed holes, routed slots and a few controlled depth routs (not right through the PCB). I used a series of hatch patterns to discriminate full depth routs from the controlled-z routs and labelled it all on a different mech layer. Board came through without fault. I have never had a slot routing error. BTW - Mike, either you are not doing many PCBs or you are much more comfortable with Protel and PCB manufacture in general. I recall you thinking not so long ago, when you started in this game, that it was all a bit of a nightmare. Congratulations. Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] irregular shaped holes ??
ian said: BTW - Mike, either you are not doing many PCBs or you are much more comfortable with Protel and PCB manufacture in general. I recall you thinking not so long ago, when you started in this game, that it was all a bit of a nightmare. Congratulations. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * thanks ian. i'm not a full-time protel person. writing digital test programs is my main job. i needed 3 boards for a interface between the board we were testing and the test bench and we had lost the person we had who did board work, so we ended up buying protel. learning protel turned me into a pcb magnet... anybody that needed one came to me. we even picked up a significant legacy job where all the spares were shot and they needed new ones built, but all they had were drawings, and no actual gerbers. i've been doing about one board every three weeks. i enjoy using the protel software and i think its a good package, even if it is a bit unstable. one thing i've found out is that there is always something new to learn. another thing i've learned is that the answer is usually here on the email group, and not in the protel documentation. grin miker * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] irregular shaped holes ??
thanks for the suggestion about putting some text inside the cutout area. one thing i tend to forget is that people do actually look at the gerbers. i get in this mode where i think all they do is blindly submit them to a machine and a pcb comes out the other end. i'll make a readme file too. miker -Original Message- From: Peter Bennett [SMTP:[EMAIL PROTECTED]] Sent: Wednesday, July 18, 2001 5:11 PM To: Protel EDA Forum Subject: Re: [PEDA] irregular shaped holes ?? Robison Michael R CNIN wrote: thanks peter, recently we acquired some gerbers for a board that had a hole in it that was used as a handle. i tweeked some of the silkscreening and sent it off to advanced circuits and they produced the board with no problem. i did call them and ask if they could do irregular holes (not pads) first. so there is evidently some sort of standard for denoting these sort of holes. unfortunately, its difficult for me to reverse engineer the former card's gerbers to see what sort of actions i need to take in protel to produce it. hmm... i've got an idea now. i went to tools/preferences/display/ and selected single layer mode and went thru the various layers and the mechanical4 is the only layer which displayed the army- green board outline. i'm gonna venture a (dangerous) guess that if i put the hole outline on this layer that it would be noted as a hole. any general consent on that? If you include Mech4 on the gerbers for the copper layers that should work. For large cutouts like that, I would also place text in the area to be removed saying Cutout 1 x 4 to indicate the area to be removed, and its approximate size, as well as mentioning the cutout in the readme file. -- Peter Bennett TRIUMF 4004 Wesbrook Mall, Vancouver, BC, Canada GPS and NMEA info and programs: http://vancouver-webpages.com/peter/index.html * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
