OSX Monterey, KiCad 7.06-0, if you change the Schematic Editor Grid to 0.1" (Similar to Eagle Default), symbols are still placed at the 0.05" grid spacing. They do not snap to the 0.1" spacing. Wires do not snap to the component, as they are on the 0.1" spacing.
If the entire spacing is 0.05", snapping works.
This happens even if you change the spacing in preferences and in the context menu on Kicad schematic editor screen.
Is there a way around this? (Using CTRL key seems to allow non-snap movements, and makes it difficult to wire to the symbol.)
symbols are still placed at the 0.05" grid spacing
I think you have not looked exactly enough. I believe the symbols centre (the anchor point, not visible in kicad) is correctly placed at the 0,1" grid. But the original standard library symbols are built with a 0,05" grid in mind. So the pins for of the original standard symbols are often placed on a 0,05" grid → this results on pins which can’t be placed on 0,1" grid in the schematic. Only for some symbols the pins are by chance on a 0,1"-grid → only these symbols work well on a 0,1" grid.
You can check this:
place Device:D (a simple diode-symbol from device-library). This will not work with your 0,1" grid.
place Device:D_Dual_Series_CAK (a double diode with middle connection, also from device-library). This will work with your 0,1" grid.
The solution is: If you want to work with a 0,1" grid: you have to build and use your own symbol library (though some standard symbols will work)
Using CTRL key seems to allow non-snap movements, and makes it difficult to wire to the symbol.
Yes, therefore use it only for text and graphically items, not for symbols, wires, busses.
If you experience grid-issues also note the RMB-click–>context-menu–> “Align elements to grid” function (only available if you have a active selection)
I believe the symbols centre (the anchor point, not visible in kicad) is correctly placed at the 0,1" grid.
You are correct.
So, the problem is that the symbol cannot be wired if the schematic is 0.1 spacing, unless of course you bring a microscope, use the CTRL key, and get very lucky.
If the symbols are created with 0.1 spacing for the pins, then they can be wired on 0.1, 0.05, or smaller spacings. That suggests 0.1 spacing should be the default for creating new symbols.
Or you change the grid to .05 in or 50 mil.
The whole schematic and symbol part of Kicad is based on 50 mil.
Don’t forget, the grid is really just an abstract number, not really a measurement. The grid could just as easily be stated in pineapples or tree leaves. There is no way to measure what is on the screen.
Changing the grid (after the fact) does not change anything which is already placed on the schematic. You have to do that yourself in a separate step. mf_ibfeew wrote down how to do it, but I think you read over that.
Set your grid to your newer preferred standard.
Press [Ctrl + A] to select everything on your schematic (or zoom out and drag a selection box around everything.)
Press the right mouse button and select: Align Elements to Grid from the context menu.
KiCad is quite strict in applying the KLC to it’s libraries. And the KLC states that the center and all pins of schematic symbols must be mapped to a 100mil grid:
KiCad is quite strict in applying the [KLC] to it’s libraries. And the KLC states that the center and all pins of schematic symbols must be mapped to a 100mil grid
Yes, the center is always mapped to the grid (as the symbol center is always at 0,0).
But there are many symbols where the pins are not on a 0,1" grid, but on the 0,05" grid.
examples:
many of the 2-pin symbols from the device-library (R, C, D, crystal)
some of the 3-pin symbols in the transistor-libraries (for instance some digital transistors like DTC144E)
I must admit that my knowledge stems from kicad v6 library, as I don’t update the libraries with kicad update. So maybe this has changed with v7/v7.99
I also admit that I would not change the library - the recommended grid (in all official kicad documentation) is 0,05" and for this the 2-pin symbols are correct. If someone wants to work with 0,1" (like wsm, or me) it’s reasonable that they have to (partly) build there own libraries.
In the end the original library is only partly useful (integrated circuit symbols mostly work well) if the user works with a 0,1" grid. Which was (most probably) ther eason for the opening post.
And the “Align to grid” function is also only partly useful:
take and place a standard R symbol (which has the pins on 0,05") on a 0,1" grid: symbol center is on grid, pins are offgrid (because pins are on 0,05")
context-menu–>align symbol to grid: symbol center is offgrid (from the 0,1" grid), pins are on 0,1" → good
But every subsequent move/Drag operation afterwards aligns again the symbol center to the grid, placing the pins again offgrid. This would require to use the “align to grid” function ever and ever again.
–>summary: working with some (many) original symbols on a 0,1" grid is not funny
KiCad is quite strict in applying the KLC to it’s libraries. And the KLC states that the center and all pins of schematic symbols must be mapped to a 100mil grid:
Hmm. That, essentially is my complaint. The 2 pin symbols in the KiCad 7.x libraries have centers on 0.1, but the pins are on 0.05. By the statement above, they violate the KLC.
So, according to the above statement, 50mil pins that do not map to 100mil grid is not according to the KLC guidelines, as the pins must be mapped to the 100mil grid.
As many have indicated, 0.05, 0.1, those are just numbers. The problems with those numbers has to do with moving between PCB packages. Others out there have other standards, they all seem to agree that 100mil is the “standard.”
Bottom line, if I work on a 100mil grid to satisfy customers, KiCad presents a problem with connecting parts that show up in the standard library using by using standard schematic wire behavior. Note, however, if all the parts followed the KLC as you described, then there would be no problem.
In the end, this issue is a tempest in a tea kettle. Not a big problem, just a time consuming one. I was just wondering about a simple work around.
All that being said, I really like how KiCad has move forward in its design. It is a bit more consistent in behavior with other packages out there such as mentor, eagle, etc.
Gosh, you’re right.
Even the bog standard resistor symbol does not conform to the KLC.
The whole KiCad project must be in ruins, what an inconsistent garbage!
Or rather, I had never noticed it before, I think I’ll just keep my grid to the standard 50mill
Although, I do admit I have a strong tendency to line up the connection points of all schematic symbols on a 100mill grid. For me it means I line them on the even grid points only. I leave many of KiCad’s settings at their default, but I do have a tendency to fiddle a bit with Schematic Editor / Preferences / Preferences / Schematic Editor / Display Options / Grid thickness and the color of the grid to find a balance between usefulness and obnoxiousness that works with the combination of my brain, monitor and eyes.
And since when does the length of the Base Pin on the humble Bipolar Transistor meet with the KLC rules? https://klc.kicad.org/symbol/s4/s4.1/ allows the use of a pin of 225 mil. in length as well as C & E pins of 100 mil? Two busted rules on one symbol
Not only is the sky falling, but the ground is raising!!!
Pin length doesn’t matter at all. Only the end connection point MUST be on grid. It looks like most of the circuit primitives have used a 0.05" grid to keep size down.
The 0.1" rule matters for IC pins to keep everything readable.
The end connections on your library parts are always on a grid: So far it is 0.05, not 0.1. (and 0.1 is the rule <grin>) Maybe change the rule. Simpler than changing the libraries.
I am amused by the amount of back and forth on this. However, with corporations and governments being arbitrarily inflexible, it might be worth making the default libraries follow the rules. Or it might not. Not my call.
The rules (which are broken in the official libraries) are not rules, because in practice they are used as guidelines that can be ignored without any consequence. (And those guidelines I happen to agree with.)
Bottom line: align component (end points) to the grid before wiring. The 0.1" grid cannot be used to place and wire components without extra steps. No big deal. Only cost is time.
Thanks! There is a work-around if you wish to use 0.1" grid, for most components. That is all I needed.
