PCB pls comment/feedback me -design by Diptrace - Page 1
Forum section: electronics / general

author: nquantum
author_rank: Regular Contributor
timestamp: January 02, 2015, 11:52:16 am
content: Circuit description:This is Step motor driver circuit by L297 and L298 IC. I plan to drive step-motor <2A maximum or I'll fry IC.For the Vref I use simple DAC R-2R resister ladder and LM385 Voltage Ref so that I can choose approx. 0.5A - 2Aso far so good... with experiment wire-lap board. So I design PCB.PCB description:-> copper thickness 1oz-> trace clearance is 12mil-> signal trace 15mil-> +5V trace 20mil , GND for +5V trace 20mil-> +24V trace (2A average) and Step-Motor trace 50mil , GND trace for this also 50mil-> Ground plane is on top layer and clearance is 12mil , remove unconnected islandI do manual route of Step-Motor trace 1st since the terminal quite far from IC but it convenience for connection for outside. (well I copy from Gecko they put all terminals at same place at front)Then is 24V trace and GND and +5V since this power line and average current is 2A so I put it quite big trace.After that I use auto-router since it quite small board and dense of component. After that I check every net , one-by-one and try to adjust not-good of what auto-router done. I only want it to find some way shorten my time. I know it not good idea to rely on auto-router. But after it done its job then I check again net-by-net to adjusts some.What is you guy thinking? Any suggestion? What error u might see which I over look?It's my 1st PCB that I use "ground plane" does it good? I'm not sure about1. I route GND finish "BEFORE" pour ground plane is it good idea/bad idea? Gonna be problem?2. I pour the plane on top layer and 12mil clearance is that too small gap?One thing I concern is 24V trace and step-motor trace I put them 50mil wide. That gonna be 2A average current and some maybe have spike current due to step-motor behavior but I think it only short time. I plan to not drive it until 2A only 1.5A - 1.7A max.If I increase copper thickness from 1oz to 2oz is it worth money?Thanks u for all comments1.schematic2.component side3.top & bottom4.bottom5.top without GND plane6.top with GND plane7.hole & pad & via

author: nquantum
author_rank: Regular Contributor
timestamp: January 04, 2015, 11:15:37 am
content: no one?

author: Rerouter
author_rank: Super Contributor
timestamp: January 04, 2015, 12:58:58 pm
content: Your layout looks sound, only thought is, how is the heatsink mounted?C9's ground is on an island, R10 is almost on an island, and the ground to U1 is not thick enough (you want him to be able to handle 4A)It appears your almost designing this thing for easy assembly / repair, the only thing out of place from being fully OCD would be rotating U3 180 degree's and pointing all the diodes in the same direction.

author: free_electron
author_rank: Super Contributor
timestamp: January 04, 2015, 01:19:45 pm
content: That 470 uf cap needs ro be right next to the l298, not half a board away.Your routing is spaghetti . It looks autorouted... . Annular rings are too small, make oblong pads under the l 298 to combat thermal fatigue.Beef up your traces for the motor. No need for 2 ounce copper. This can be routed perfectly clean.Pit the motor output comnectors at the other side of the board, close to the l298

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 04, 2015, 02:35:28 pm
content: I don't see any stitching at all?Follow the path of the ground fill. I see three main... peninsulas, for lack of a better term. Yes, they all connect up electrically on the right hand side (referring to #6), but they're completely cut apart where they're needed together the most: at the switching chip!If you pour the top side, and add stitching vias periodically along either side of cuts (traces) in either pour, you can get much better results. Place vias following this condition: at any given point on the board, try to minimize the distance to all nearby ground edges. Thus, a long trace should be stitched over periodically, because it cuts between two edges of ground on its layer. And so on. You may not be able to provide 100% coverage (meaning, every pad or trace is surrounded, above, below or side to side, by copper on one or both layers), especially where there are a lot of pins coming together (like at the ICs, where you may inevitably have to deal with nets other than ground being above and below each other at some points), but those can all be easily minimized on a board with a density like this.Alternately, you can try to avoid running long traces on the bottom as much as possible, swapping between layers frequently if necessary. So the bottom side copper remains as solid as possible. But a stitched board is far superior, well worth the effort.Tim

author: mariush
author_rank: Super Contributor
timestamp: January 04, 2015, 02:44:08 pm
content: Wouldn't it make more sense to rotate the DIP IC 90 degrees? Seems like that would fix a lot of traces and simplify routing.Did you consider using double common anode or dual common cathode diodes instead of those 8 individual diodes? It's a bit more expensive but they're available in to252 or to-220 (and other packages that take less space) and they'd be better heatsinked compared to 4 separated diodes standing freely in air. With to-220 you could also move them to the sides and maybe use some strip of aluminum or copper to cool them (if not screwing them on that large heatsink with some insulation)I'd also suggest you stop being afraid of surface mount components and use 0805 resistors and capacitors. A good candidate for this would be those leds for those 3 resistors limiting current, lots of wasted pcb space there... i'd also change the layout so that the ground for all three leds would be in one line, simplifying the whole layout.Agree with the previous suggestion of having the large capacitor closer to the ICs.

author: DerekG
author_rank: Frequent Contributor
timestamp: January 12, 2015, 10:43:00 am
content: If you are going to build a lot of these, you can save money by using 2 x 6 way screw terminals rather than 6 x 2 way. This will also speed up assembly.I avoided SMD designs for quite a few years, but bit the bullet in ~2000. It was the best decision I ever made. Let the robots do all the laborious work. SMD components are now often quite a lot cheaper than through hole & many new components are only available in SMD.One of the design advantages of using SMD components is that they are mounted only on one layer (generally the top layer). This leaves the bottom layer much less busy which allows more room for thicker, current carrying tracks (remember that you can open up the solder mask so that the wave soldering adds to the existing copper thickness).Another advantage is that you can open up the solder paste screen to add solder around SMD components for heat sinking purposes. This often means that you no longer have to install a metal heatsink.I have recently completed a photovoltaic controller using 2 x high voltage mosfets in parallel. Each mosfet is mounted on a connected, symmetrical top layer 3oz copper pour, making up about 60cm square. Solder paste is then added to this large copper pour in a grid fashion (to avoid excessive bubbling in the infrared reflow oven).This has proven cheaper, faster & more efficient at removing the generated heat than installing metal heatsinks.The circuit board holds numerous connectors & LEDs etc in specific locations to suit an existing plastic moulded box. This meant that the circuit board needed to be relatively large, regardless of how many components were going to be placed on it.Added: All the above was completed in the latest version of DipTrace, however I could have designed it in either Altium or Proteus.Also, consider widening the tracks where they leave the ICs (& other components), particularly on the top layer. You can neck the tracks back in once a few mm from the component.If you leave the thin tracks on the top layer (under the ICs), you will likely rip some off the board during any rework/repairs.