I would agree with his statements.. but there is other equally important considerations.
First thing is use the component centre as the component origin. It will save you headacks later, Place it on a metric (1mm) grid even if the rest of the board is placed on an imperial grid. (But move your board origin to 2000mil, 2000mil first). Place the vias on a 0.5mm grid. Increase the pad size slightly 20mil? .. unless you have a doc to say otherwise and vias to 20mil with .3mm hole.. that's 8mil annular ring and will be less likely to break out. Also the tracks on the top 8mil. it fits ok.. except around the edge where they will need to be 7 mil to keep 8mil track to track spacing (you may want to neck down) this will give you less of a problem with under/over etch. Then identify all the ground and power traces, they will dictate how you layout the whole device. I have used a XXX type arrangement for the grounds before, this seems to work well (that is you join all the grounds with long diagonal traces and place a via at the intersection of the traces). This is a Motorola thing not mine :-) Power is usually after the GND and uses the free space created by the GND XXX for its vias.. makes it easy to see on the bottom of the board too. The you have to look at your signals as suggested, and determine how many layers you will allow to route out on and how many of the signals are high speed, matched impedances, time critical, slow speed, static etc. Do the grid, via and traces and identify the power/GND and I will look again :-) as will others I am sure Simon -----Original Message----- From: JaMi Smith [mailto:[EMAIL PROTECTED]] Sent: Saturday, 28 September 2002 7:03 a.m. To: Protel EDA Forum Cc: JaMi Smith Subject: Re: [PEDA] 1020-pin BGA out-routing question (some add) Juha, Just looked at your database. First, your vias are misplaced, and need to be exactly in the center of the opening between the pads, which appear to be on a 1mm grid, which means that you vias should be on a .5mm grid. This will keep your vias as far as possible from the actual BGA pad, and you want as much here as you can get. This wili also allow you to use a bigger via (see below). Secondly, you will possibly want a larger pad to drill ratio on your vias if at all possible, to prevent massive breakouts, which while acceptable by some standards. may be excessive with that current ratio. One of "routing" numbers being batted around by some board houses is somthing they call the "five fours", which is three 4 mil gaps with two 4 mil traces, all between a 20 mil pad with 10 mil holes for 40 mil spacing on a BGA. If your spacing on the BGA is actually 1mm, which is .03937 . . . , instead of 40 mil, then you have to slightly adjust the size of the pad, and everything else will fit. Even here you are gonig to possibly see breakout, which once again is allowable, providing that you are using "teardrops" for all of your pad entries. How big is your board anyway, overall size wise. The above numbers are based on "standard" alignment of all features within 5 mil, and unless your board is fairly large. everything seems to be very do-able with out too many layers, or the need to go to micro vias, or ever to blind or burried vias. JaMi ----- Original Message ----- From: "Juha Pajunen" <[EMAIL PROTECTED]> To: "Protel EDA Forum" <[EMAIL PROTECTED]> Sent: Friday, September 27, 2002 1:09 AM Subject: [PEDA] 1020-pin BGA out-routing question (some add) > Hi again, > > <> What is the best PCB layer stack for > this type of BGA? <> > > http://groups.yahoo.com/group/protel-users/files/junk/ > > There is 1020-pin 1mm pitch BGA. It would be very > pleasing to have some information and help how to > route that huge BGA. What are trace width and cap > between different tracks and so... > > It would be very nice if you couldedit that file > (how to route it) and then send it to me to this > addrss [EMAIL PROTECTED] > > I really need all useful information > about routing this BGA! :) > > > Sincerely, > Juha Pajunen, Hw Engineer > Bitboys Oy > E-mail: [EMAIL PROTECTED] > ------------ > NOTE: This message, and any attached files, may contain privileged or > confidential information. It is intended for use only by the designated > recipients. Any disclosure, copying or distribution of, or reliance upon, > this message by anyone else is strictly prohibited. http://mobile.yahoo.com.au - Yahoo! Messenger for SMS - Always be connected to your Messenger Friends * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://email@example.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *