On 13 Apr 2007 at 12:02, PicDude wrote: > On Thursday 12 April 2007 19:57, Brent Brown wrote: > > Hi, > > > > Because it's round then you don't have much choice except a routed > > board outline! Vee-groove can only do straight lines and lines must > > go right across the panel (can't start and stop). > > Actually, V-groove could've worked since I don't mind a few straight > sections around the circle. But I still can't use it for the other > reasons. > > > > I've done a similar board/panel (boards were 34mm diameter). Four > > breakout areas or "bridges". Each breakout area is two 0.8mm drilled > > holes ... > > Sounds good. > > > > Other general tips for panels: > > > > - Leave room for panel to be held in assembly jig. Typically a 10mm > > "salvage" strip at least on top and bottom edges of panel, often on > > all 4 sides to increase rigidity of board. > > That's seems to be about the size of the ones on the current panel I > have (which was panelized by a CEM). But there are only 2 side rails > on this one -- see here... > http://narwani.net/neil/stuff/Panel_2x5-b.jpg > > > > - Put a mounting hole in each corner of the board for the assembler > > to use. I typically use 4.1mm unplated holes and locate them on the > > salvage strips. > > Ah-ha! This is exactly the type of info I need. I see holes in the > corners -- is 4.1mm a standard or common size? I don't know exactly, but I've standardised on it myself and it's been ok with 3 different manufacturers. > > - For machine assembly each board must have "fiducial" marks for the > > pick-n-place machine to register to. Usually 3 marks so it can't get > > the board round the wrong way. Fiducials are usually a round pad > > with solder mask relief to increase contrast. Bottom left fiducial > > makes a good x=0, y=0 reference for pick-n-place coordinates. If > > components are on both sides of the board then you need fiducials on > > both sides. Very fine pitch components may need their own fiducials. > > Also put fiducials on the panel, usually on the slavage strip. > > On my individual PCB, I originally had a small fiducial (so 10 > available on a full panel), which the CEM said they would not use. > Instead, they put their own on the rails. Again, is there a > "universal" size that most places can work with? I see Eagle has > circles, squares, cross-hairs, etc. Not sure if all CEM's can work > with all of those. A good size seems to be a 1.5mm diameter pad, and a 3mm diameter "hole" in the solder mask. 1mm pad and 2.5mm solder mask hole are good for component fiducials, eg. placed in two corners of a QFP footprint, but I think is close to the minimum size that can be used. > > - Size the panel to best suit your assemblers requirements and PCB > > manufacturers capabilities. Assemblers don't like panels too big as > > they flex too much. > > This 4.5" x 10" size (full panel) is relatively small I'm sure. I > would like to remove the "bridges"/supports on the sides of each > circular board so that it's only supported by the upper and lower > bridges. This is to make it breakaway easier. Not sure if that will > cause a problem, but I would think/hope not, as the 2 long side rails > will provide horizontal rigidity and the bridges on the upper/lower > side of each circular board will provide vertical rigidity. A rule of thumb is panels should be about A4 (210 x 297mm) size or smaller. As for reducing the number of bridges it's border line but I suggest that less would be insufficient. What you have now is good. > > - Protel/Altium Designer has a "place embedded board" function, that > > inserts a PCB file in a step and repeat fashion, you specify the > > spacing, rotation, number of x and y steps. Panel file is linked to > > PCB file so any updates are reflected. Eagle and other CAD programs > > may have something similar. Else you are stuck with copy and pasting > > which is time consuming, makes really big files, and can often have > > issues with duplication or incrementing of component designators. > > IIRC there is a script for Eagle that automates the panelization as > you describe, but the cut/paste process is simple enough that I > haven't bothered. > > > One other thing I am wondering about is specifying the routing lines > -- if I place a line (using the Milling layer) for the board-house to > route along, they will *center* the cutting-bit there, rendering the > individual boards too small. Is there a standard cutter diameter I > can calculate/compensate for? Or can I specify the cutter size? As with lots of things, it depends on the PCB manufacturer you use. In my experience if I specify a line and say that it is the board edge then the manufacturer can use whatever cutter size they like. If you can find out what their standard or preffered cutter size/sizes are then that helps a lot. When some particular detail demands a certain tool size then I specify that, eg. 1mm, and provide two lines (on different layers) - the edge line and the centre line for the tool to follow. > > Hope this helps! Brent. > > Tremendously! Thanks, > -Neil. > -- > http://www.piclist.com PIC/SX FAQ & list archive > View/change your membership options at > http://mailman.mit.edu/mailman/listinfo/piclist > -- Brent Brown, Electronic Design Solutions 16 English Street, St Andrews, Hamilton 3200, New Zealand Ph: +64 7 849 0069 Fax: +64 7 849 0071 Cell: 027 433 4069 eMail: brent.brown@clear.net.nz -- http://www.piclist.com PIC/SX FAQ & list archive View/change your membership options at http://mailman.mit.edu/mailman/listinfo/piclist