Why Rounded rectangular pads are used in place of rectangular pads KiCad footprint library?
Because we follow IPC-7351C
Reasoning behind choosing rounded (other than just following the standard, probably behind the standard, too):
- If you look with a microscope, rectangles aren’t really rectangles in etched board, the corners are rounded anyways because of the etching process.
- Rounded corners give more room for positioning and routing – important when 0402 and especially 0201 components are used if space is at premium.
- Rounding doesn’t affect negatively to assembly or anything else.
I have read that the solder paste tends to stay in the corners of the template.
The general goal of IPC is to allow users to easily switch their manufacturers. So very high on their list is to improve portability and reduction of manufacturer dependent variables.
Reasons i remember as stated in IPC:
- Rounded corners in stencils improve manufacturability (less process dependency as you define the radius not the tool used).
- Also for stencils rounded corners improve how well the paste is released from the stencil (I did not fully understand the physics behind this but i assume a lot of testing was involved here).
- Rounded copper improves the surface tension behavior and therefore flow behavior
- IPC never ever suggested the use of pure rectangles and only suggested the use of oval because of a lack of support in the more popular design tools. (They now expect every tool to support rounded rectangle which is why they suggest it for future use)
Because we follow IPC-7351C
Just a couple of notes on this
- IPC-7351C is not released and might not be
- IPC-7351 is now just guidelines and they recommend following the manufactures outline
https://www.pcblibraries.com/forum/ipc7351-or-manufacturer-recommended-footprint_topic2639.html (Tom H is the author of IPC-7351)
Shame, I have been pushing for IPC-7351C footprint where I am for quite some time and why? (ie OP question)
- As someone that deal almost exclusively with higher voltages rounding everything is a must to minimise charge buildup. Pads, traces, planeshapes…
- IPC-7351C were advocating rounded due to experience with lead-free where the resulting fillet provided improved adhesion
- They look nice
I found my email where I 1st started advocating this with a link back to PCBlibaries: https://www.pcblibraries.com/forum/rounded-rectangle-pad-shape_topic1462.html
Better stencil release and paste mask stencil apertures are normally corner radius
lead-free doesn’t generally flow into the corners
There were contradictions in the spec where the pads were oblong but tools could only do rectangle. These days tools can do rounded rectangle
rounded rectangles aligns better with manufacture processing
rounded rectangle pads strengthen the solder joint
it looks nice !!!
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.