I have built a foot print to link up with a four connection shunt for current sampling.
This was done by creating a non standard pad. This was done by placing a small pad and laying my shape of pad on the top and then selecting make pad as per instructions in blog.
The foot print looks ok to me with copper, paste and mask. All three I can turn off and on.
But when I place an area of pour, as you can see from the screen dump the pour does not connect.
A trace can be placed but connects at the point where the small pad originated.
Suggestions would be appreciated
Thanks
In V5 custom pads doesn’t support thermal relief. I would suggest editing the fill of the footprint to “solid” instead of “use zone properties”. You can also change this in the FP editor to avoid doing it every time
1 Like
Or keep it as none and make thermals manually.
In general: why use custom pads for such a simple rectangular pad?
Thanks for your assistance that worked a treat!
In general: I didnt realise that it was such a simple rectangular pad ! Given that there is the small rectangular pad sticking into the side of it. Will look forward to a demonstration of how else to due the job.
By the way the symbol was from the standard library and I finally gave up on trying to find its partner in the footprint library. Hence my attempt at what you see.
The foot print was prompted by the application example given by Bourne and the Kelvin Principle of measurement.
Just yesterday (5.1.2) I was trying to change in Footprint Editor in Footprint Properties the “Connection to Copper Zones” from “Use zone settings” to “Solid” and it has no effect.
When trying to report a bug I found:
@Shack was referencing changing it on a per pad basis not for the full footprint.
In this case the pad is automatically set to none as it is a custom pad. This will always overwrite the footprint settings! So changing it at the footprint level would not have an effect anyways. This is unrelated to the bug you reported.
–
Would require you to share at least the exact part number or even better a link to the datasheet. (Plus me finding some time to look into it. Right now i suspect you might have misunderstood the manufacturer suggestion as there are simpler ways to get a 4 wire connection realized. To be honest this mostly comes from my experience reviewing similar footprints on the kicad library repo. 80% of contributions have at least one major error or misunderstanding of the manufacturers suggestion. And from the 20% that get at least this correct 80% have some KLC violation leaving only a very small amount of self made footprints to be first time right. It is a lot better for scripted footprints where it is about 90% first time right.)
Ironically I was the one who made that bug report 
Are you sure?
Who decided that short posts are not allowed and I have to add something?
Ok shack indeed made an error here. (And my brain automatically corrected it without me realising it. So I screwed up as well.)
https://www.mouser.co.uk/datasheet/2/54/ss2h-3920-935112.pdf
this is the link to the component data sheet
This is the link to the application note that prompted the layout that used for the foot print. and yes there are differences between the data sheet and application sheet.
Far be it for me to add to your work load, but I would be interested in your thoughts on the matter!
You wrote in your first message
Here’s the corresponding application note:
It’s very forgiving, you just need four rectangle pads two larger for current, two smaller for sensing pad. Typically you connect the current pads to zones, therefore the pads seem to continue to larger shape.
If you use a 2-terminal one it even simpler, just two rectangle pads from where the traces go from between the pads.
1 Like
You will need to create a new component with 4 terminals (both symbol and footprint). Each “pin” will be independent. Do not be distracted by the simplicity of the device. While there is a DC path thru the component, there can not be shorts in the footprint.
Pin
1 DC-In Big pad
2 DC-Out big pad
3 Sense-1 small pad
4 Sense-2 smell pad
When you connect to this in the schematic, there will be 4 independent nets, as there should be in a “classic 4 terminal” measurement.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.