I’m making a footprint for this level shifter and in the recommended pad settings they spec a solder mask aperture that is -0.05mm on the y axis and 0.0mm on the x axis. PCBNew allows for arbitrary mask and paste values in Pad Properties > Local Clearance and Settings, but I can only set the X, Y dimension with one value. Is there any way to isolate the X and Y paste clearances to different values?
You will need to make a separate paste only pad to get this done.
Disable the paste layer on the normal pads and add a second paste only pad on top of each of the normal pads.
(Paste only pads should not have a pad number assigned)
Which package are you working with? In my 30-second scan of the datasheet, I didn’t notice the assymetry you describe.
I have never encountered this situation so I can’t give specific advice. I have only worked with some of the larger SMD packages (SOP, SSOP, etc) where the paste lay-down has a fair amount of leeway. In my experience, the paste pattern is almost as much a function of the manufacturing process as the actual package dimensions. (I.e., I’m accustomed to manufacturing engineers telling me, “Hey, we need a little more paste here and not so much there.”, regardless of what the component manufacturer suggested.)
Having said all that . . . have you tried to define a footprint with custom paste aperture specifically for your part? As you know, KiCAD lets you define some rules for automagically generating the paste stencil but I believe it’s possible to over-ride them on a footprint-by-footprint, or even pad-by-pad basis.
The TI_DQE package seems to show exactly what the OP was questioning.
Personally, even though I have yet to have a board populated, I fully expect that it won’t really matter if there is more/less solder paste in one vector or another as once it gets hot enough it will flow over the pad and part leads.
Hey thanks for the quick pile-on!
@Sprig you are right, I’m working with the DQE footprint, aka XSON8.
@Rene_Poschl I think your solution is winning. I can see that when I am initially designing the pad, I have option to include or disclude the paste layer. Also, I can create a ‘pad’ that only exists on the paste layer.
Just did that and it took on the order of about 2 minutes. isolating layers, I can see that it seems to be working. Will have to inspect the .gbr to verify, but that seems to have fixed it!
Yeah, that’s my understanding for about 99% of cases. I’m not a manufacturing guy but apparently there are situations where you might adjust the paste pattern based on the direction reflow heat gets applied from, or nearby components that create a “shadowing” effect.
My understanding is that the primary factor is the total volume of solder paste deposited on a pad, and its exact location on the pad is a secondary consideration. When you watch a reflow process in operation it’s sort of sexy to watch the solder liquify, then parts dance around as surface tension, solder mask, and the components’ mass encourage everything to line up. (OK, “sexy” is in the eye of the beholder and I may not think of reflow soldering in terms of parts squirming around to get a good alignment if I was in my 20’s or 30’s.) The volume of solder paste, in turn, is affected not only by the paste aperture but also by the stencil thickness, solder paste consistency, and temperature in the production area. That’s why PWB layout software typically uses a global “Paste Mask Shrink” parameter, often not defined until Gerbers are generated, to customize the paste stencil for a particular production environment.
Yes. I overlooked that when I did a quick flip-through the datasheet.
For your own future reference, AFAIK this is how the standard library handles center pads that need multiple smaller paste zones to avoid floating the chip up on a drop of solder, pulling the perimeter pins away from their pads. I suppose if you really wanted you could create a symbol as a custom pad that is on paste only as a hidden easter egg that only the stencil handlers and paste inspectors will see.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.