[psas-avionics] min trace width
Hi all, I'm working on the the APS board and I was just wondering what the min. trace width should be. One of the ICs I'm using is a 3mm x 3mm MSOP-10 (TPS2490 hotswap controller) and the lands are narrow and close together meaning if I use the default 0.016'' trace width, I get a keepout error. Are 0.01'' traces wide enough? Thanks! Scott ___ psas-avionics mailing list psas-avionics@lists.psas.pdx.edu http://lists.psas.pdx.edu/mailman/listinfo/psas-avionics
Re: [psas-avionics] min trace width
Hi Scott, In dealing with trace width, here are a couple of things to consider. 1) Temperature rise, current, voltage drop, arc resistance (for higher voltages), and impedance (for transmission lines); and 2) Fab capabilities. For the first one, you likely know the current going through the traces, so you only need to decide what is an acceptable temperature rise for the trace. This rise is the temperature of the trace above ambient temp. 10-20 degrees C would be a lot of temperature rise unless you are building a high power circuit. http://circuitcalculator.com/wordpress/category/calculators/pcb/ look down the list. There are other handy calcs for power dissipation as well. For the second one, Check with your PCB Fab house and see what they are capable of doing. I generally add a little insurance by *not* going all the way down to the minimum trace/space dimensions that they are capable of. Instead, make your minimum a couple of mils bigger than theirs. For low power signals, it's not uncommon to see 0.007 traces. Also, remember that a low frequency (slow rise/fall time, or analog) trace can be 'necked down' (reduced in width) just where you need it for some applications, but don't try that with fast signals. Quoting Scott Schuehle scott.schue...@gmail.com: Hi all, I'm working on the the APS board and I was just wondering what the min. trace width should be. One of the ICs I'm using is a 3mm x 3mm MSOP-10 (TPS2490 hotswap controller) and the lands are narrow and close together meaning if I use the default 0.016'' trace width, I get a keepout error. Are 0.01'' traces wide enough? Thanks! Scott ___ psas-avionics mailing list psas-avionics@lists.psas.pdx.edu http://lists.psas.pdx.edu/mailman/listinfo/psas-avionics
Re: [psas-avionics] min trace width
(2009.05.19) scott.schue...@gmail.com: I'm working on the the APS board and I was just wondering what the min. trace width should be. One of the ICs I'm using is a 3mm x 3mm MSOP-10 (TPS2490 hotswap controller) and the lands are narrow and close together meaning if I use the default 0.016'' trace width, I get a keepout error. Are 0.01'' traces wide enough? Thanks! Hmm, Firstly, we are using sunstone quickturn http://www.sunstone.com/products-services/product-comparison.aspx http://www.sunstone.com/pcb-capabilities/manufacturing-capabilities.aspx So the literal answer wide enough is 6 mil. However, generally wider = better. For smd components usually the trace should be no wider than the width of the surface mount land. Most msop packages have 0.4 mm wide lands. (All the cool kids avoid inches if the packages aren't in inches.) If your msop has 0.4 mm lands, then a 16 mil trace (0.4 mm .= 15.75 mil) should work. Of course some msop's are ultra short, etc. Ah, i checked and your part (tps2490) is a 0.5 mm pitch package, so your lands are probably narrower. Generally, 0.4 mm is good. power paths should be wide, see the old APS or do a voltage-drop calculation. If you need to drop down to 0.2 mm in places, that's fine. I don't think you'll need to go finer than that. ___ psas-avionics mailing list psas-avionics@lists.psas.pdx.edu http://lists.psas.pdx.edu/mailman/listinfo/psas-avionics
