When creating your board in Eagle, whats the best way to route a trace into the pad under a component? Does it matter where the trace enters, or how large the trace is? Since I make my own prototype boards, I don’t have a solder resist layer and i’m afraid that the component may tend to slide off it’s own pad if the trace does not enter at the very end of the pad, or if it’s very large.
I have only done 2 or 3 smaller SMD boards so far with my own reflow oven, and they turned out pretty good, but this next board I am working on has even smaller components, and I hate wasted board space so I try to cram everything as close together as possible without them being so close that it could cause problems when placing components or reflowing it in the oven.
As you get into the smaller pitch sized SMD components you may want to look into getting boards fabbed. Not sure what your referring to pad under a component unless your trying to mount a BGA. for these you will definitely need the mask and in most cases microvias in pad depending on the pitch of the BGA. i have dealth with the mother of small ass BGA’s the Qualcomm MSM chipset and what a beast @ 476 pins x 5 mil pitch. talk about microvia hell. If the pad is a ground then just ground it with vias. any chance you can elaborate on the Chip in question? I realize you produce your own PCBs as i did a long time ago. Since this being a SFE forum i prob cant tell you about the fab house i use since its NOT BatchPCB. but they are out there.
When creating your board in Eagle, whats the best way to route a trace into the pad under a component? Does it matter where the trace enters, or how large the trace is? Since I make my own prototype boards, I don’t have a solder resist layer and i’m afraid that the component may tend to slide off it’s own pad if the trace does not enter at the very end of the pad, or if it’s very large.
Take a look at the [Altron Inc Board Design Guidelines, pages 34-35, “CONNECTING TRACES TO COMPONENT LANDS WHEN USING SOLDERMASK” and “CONNECTING TRACES TO COMPONENT LANDS WHEN SOLDER MASK IS NOT USED”. This is a really great document to use as a baseline for PCB design rules of thumb. It’s definitely worth reading through.
jdraughn:
I have only done 2 or 3 smaller SMD boards so far with my own reflow oven, and they turned out pretty good, but this next board I am working on has even smaller components, and I hate wasted board space so I try to cram everything as close together as possible without them being so close that it could cause problems when placing components or reflowing it in the oven.
What size of SMD components are you using? Are you etching your own boards? I have found that for simple boards with few through-hole vias required, it's still worth it to etch my own boards sometimes, but check out Laen's OSH Park PCB service as well, especially if you want to do more complex stuff or just want the higher quality of a professional board. I'll jump right out and say I think it's better than BatchPCB in general. Quick turnaround and unbeatable quality.
If you are making PCB’s to hand assemble then it does not matter a lot which way you enter the pad, however if it is to be mass produced and use a reflow oven then thermal balancing has to be considered.
You can route your boards completely differently for when hand assembling than if being mass produced, there are more design rules to consider then.
For traces smaller than the pad it wont have much effect which direction you enter. For larger traces it will cause problems, in your case because you don’t have a mask. (you could get a masking pen too.) With a larger trace I would enter the pad in line with the component. This way you don’t have to worry about the component drifting left or right down the trace. It doesn’t have to be a very long segment either. Just enough to make sure the component doesn’t have options.
Not sure if SFE sells masking pens but here is one a quick google found:
Grimfox:
For traces smaller than the pad it wont have much effect which direction you enter. For larger traces it will cause problems, in your case because you don’t have a mask. (you could get a masking pen too.) With a larger trace I would enter the pad in line with the component. This way you don’t have to worry about the component drifting left or right down the trace. It doesn’t have to be a very long segment either. Just enough to make sure the component doesn’t have options.
Not sure if SFE sells masking pens but here is one a quick google found:
I saw a hack on Hack-a-Day where someone used Kapton tape to solder-mask the traces around a QFP package before soldering. You could cut Kapton tape into smaller pieces to mask traces around discrete SMT components like chip resistors and capacitors as well.
The trace width should be proportional to the expected current running through it.
0.010" = 0.3 A
0.015" = 0.4 A
0.020" = 0.7 A
0.025" = 1.0 A
0.050" = 2.0 A
0.100" = 4.0 A
0.150" = 6.0 A
Traces less than 12mils should avoid right angles, etc etc, but that’s outside the scope of what you’ve asked.
When creating your board in Eagle, whats the best way to route a trace into the pad under a component? Does it matter where the trace enters, or how large the trace is? Since I make my own prototype boards, I don’t have a solder resist layer and i’m afraid that the component may tend to slide off it’s own pad if the trace does not enter at the very end of the pad, or if it’s very large.
I’m uncertain what your board will do, but if you’re using ICs sensitive to noise (i.e. precision op amps) then don’t run any traces under the component. The slight capacitance/inductance caused between the IC and the trace(s) will be enough to dirty your signals. This also includes planes, power or ground.
The solution: Create a rectangle under the IC and apply it to layer 41 (tKeepout). This way, if you use an auto-router, it won’t route under the IC on the top copper layer. If you route manually, it’s an extra fail-safe. Create another rectangle, overlay it on top of the first rectangle, and apply it to layer 42 (bKeepout) for the same thing to the bottom copper layer.
The above is only for sensitive ICs. Things like microcontrollers and 232s are fine with traces running beneath them.
