[Bug] Footprint Editor: Pad Properties: Custom Pad shape

Description

Steps to reproduce

1. open kicad
2. open pcbnew
3. open the footprint editor
4. create a pad with a custom (rectangular base) (for this chip)
5. 

As the pad shape is Custom you should not be able (in my point of view) to define Pad x/y size, otherwise it looks like this:

vs

where Pad x/y size are set to 0.

So the cleanest solution might be to disable Pad size X/Y when Custom pad shape is selected.

KiCad Version

Application: KiCad Footprint Editor x64 on x64

Version: 7.0.6-rc3, release build

Libraries:
	wxWidgets 3.2.2
	FreeType 2.12.1
	HarfBuzz 6.0.0
	FontConfig 2.14.1
	libcurl/7.88.1-DEV Schannel zlib/1.2.13

Platform: Windows 10 (build 19045), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
	Date: Jul  3 2023 05:13:34
	wxWidgets: 3.2.2 (wchar_t,wx containers)
	Boost: 1.81.0
	OCC: 7.6.3
	Curl: 7.88.1-DEV
	ngspice: 40
	Compiler: Visual C++ 1936 without C++ ABI

Build settings:
	KICAD_SPICE=ON

added 7.0 priorityundecided statusnew labels

follow-up issue: as now solder paste margin will always be larger than pad..

follow-up issue: origin of custom pad is not in the center:

it seems to be in the top-left corner, probably at the first defined point

74AUP2G08GX.kicad_mod

I didn't finished the footprint, this is the current state:

As there are multiple, but connected things:

• the custom pad shape consists of the base pad plus (maybe multiple) additional shapes. So the x/y-size of the base-pad is usefulan should not be restricted. The user is responsible to set the base-pad (size + origin) according to the needed geometry.
• pad-size must be > 0 (set x=0/y=0 is not allowed). This is also required for the base-pad of a custom shaped pad
• if "solder paste absolute clearance" > pad-size (in your case: base pad size) than you get the warning from your second post ("no solder mask will be generated"). It could be discussed if this check is too simple for a custom shape (where there is usually more copper than only the base pad). I would recommend a dedicated issue for
• origin of custom pad == origin of base-pad - in your case the base-pad of custom pad is placed at -0.14/0.44 - this is the top left corner of the custom pad. Taking the "geometric center" as origin may be a good idea in your case, but will not work on complex shapes (think a spiral)

@mf_ibfeew thanks for your detailed answer

the custom pad shape consists of the base pad plus (maybe multiple) additional shapes. So the x/y-size of the base-pad is usefulan should not be restricted. The user is responsible to set the base-pad (size + origin) according to the needed geometry.

I was not aware of that (and I didn't checked the manual :-(

(Edit: there is not much written https://docs.kicad.org/7.0/en/pcbnew/pcbnew.html#creating-and-editing-footprints)

origin of custom pad == origin of base-pad - in your case the base-pad of custom pad is placed at -0.14/0.44 - this is the top left corner of the custom pad. Taking the "geometric center" as origin may be a good idea in your case, but will not work on complex shapes (think a spiral)

I agree, makes sense together with your first sentence.

I managed now to draw the copper outline of the pads:

Now I discovered that the two settings for the "Solder paste absolute/relative clearance" have no impact on the solder past when a the Pad shape is "Custom (rectangular base)"

Solder Mask seems to work:

74AUP2G08GX_v2.kicad_mod

something else I found out:

for the custom shape primitives the line width has to be extremely small, otherwise not the expected polygon is created:

0.2mm vs 0.0001mm

mentioned in issue #15110 (closed)

I managed to get the footprint finished, solder paste issue remains

74AUP2G08GX_1357_custom_pad.kicad_mod

To fix your footprint-pads now: On all custom pads set the base pad size > solder paste absolute clearance. Currently solder paste absolute clearance == -0.01 --> so pads must be bigger than 0,011x0,011mm. Additionally you havee to move the pad into the middle of the custom shape, otherwise this small 0,011x0,011 rectangle will stick out at the top left of your custom pad (to be honest this small stick-out copper is also not important, could very well be ignored).

I still recommend to open a dedicated issue for the paste-topic, I fear it will get lost as part of these long mixed up thread.

thanks for your tips @mf_ibfeew I just opened another issue for the still not working solder paste mask reduction on custom pads.

let's move the discussion over there

#15125 (closed)

mentioned in issue #15125 (closed)

closed