In the official KiCad Libraries I find SMD footprints with (sharp) rectangles and rounded rectangles.
For example Package_TO_SOT_SMD has SOT-23 with round rectangle pads and SC-59 with sharp cornered pads.
I did not find any information in KLC whether to use round or normal rectangled pads.
Is there a preference or standard in IPC?
Is relative or absolute roundness preferred?
My EMS is always asking me to use rounded rectangles when generating the Gerber for solder paste stencil. They say it’s about solderpaste getting stuck in the corners…
So when the part from the official library has sharp corners I usually make a new footprint in my private lib, because post processing / filtering (by the way a great feature of KiCad) can get overwritten when updating the PCB from the Schematic without carefully checking the settings.
The preference is rounded and this aligns to aspects of the IPC.
There are some footprints that are sharp corners either due to legacy or due to exceptions (thermal pad for instance ).
Most SMD items should have rounded pads. If you find square pads in the library, these are usually some old footprints that haven’t been updated or ones that don’t follow the IPC rules and have been created manually (for example the “_Handsoldering” variants).
Ok, got it!
When generating pads with different size they look strange when I use relative roundness (i.e.25%).
Parts look better if the same radian is used for all pads of a footprint.
Is there any recommendation from IPC for preferred radian?
In Kicad 7.0.1 release build the footprint wizard is also still using rectangular pads (at least for [SOIC] ).
There are no requirements or standards for rounding in the ipc standard… there are recommendations and nothing more… rounding everything is a bad idea… I don’t even understand where this theory came from that everything needs to be rounded…
indicate the number, if possible, which says that the platforms must be rounded?
Sorry, I’m just a hobbyist and I don’t have the professional books and specifications. I’m just following what you can find on the internet, for example here: pcb design - Should SMD footprints be rounded? - Electrical Engineering Stack Exchange
I have a personal rule to have a corner radius of either 0.25mm or 25% whichever is smaller.
Pad size of 0.6mm by 0.6mm at 25% has a corner radius of 0.15 - keep using 25% corner radius.
Pad size of 1.5mm by 1.5mm at 25% has a corner radius of 0.375 - too much, manually reduce to 0.25mm.
Please note that this is based off of anecdotal evidence that rounded pads have less issues with wetting of the whole pad, also it’s a bit easier to route tracks around corners and it doesn’t compromise much of structural integrity of the solder joint.
if you look at what is written there, we are talking about lead-free solder… there is no ban on rectangular pads… if you are not sure exactly why and how much you need to round and where… then you can contact the manufacturer, they usually have recommendations for the shape of both the footprint and the stencil aperture… There are two more important points… 1 rounding reduces the contact area 2 due to the peculiarities of printed circuit board production technology, in any case, your corners will be rounded to a small radius… (features of etching printed circuit boards)
I suggest you go read IPC-7351A and IPC-7351B
I suggest you read this yourself… and also follow the recommendations of the manufacturer of specific microcircuits and parts and not round everything off indiscriminately… I repeat once again, there are no requirements for rounding all footprints, there are only recommendations…
Many thanks to all who have contributed to my question. I have learned a lot and have a clear view how to design new components.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.