Hi,
KiCAD Newbie here. Been using OrCAD, PADs, Logic, DxDesigner and Altium for 45 years. Learning how to spell schematic right now.
When I move a symbol I really want pins to stay on grid. For me that is 100mil. If a symbol dimension is not a multiple of 200mil moving by a centroid gets pins off grid. I need to be careful to select a pin when starting a move. Seems the Altium and OrCAD move defaults to a pin when I start a move, great.
The other edit functions is rotate which rotates from the centroid, that is good.
Is there any setup for grids that helps preserve pins staying on grid other than just the size of the symbol?
Kicad library symbols are designed for use with a 50 mil. grid. If you change your schematic grid from 100 mil to 50 mil you should not suffer “off grid” problems with Kicad symbols.
An easy way to change your grid is to Right Mouse click on an empty space of the worksheet, Left Mouse click select Grid from the list in the pop-up box, scroll through the grid settings to find 50 mil then Left click that setting.
There is much information here, particularly the “Getting Started” for basic Schematic use.
I have never (using KiCad since 2017) noticed it.
I’m working with 50 mils grid (KiCad default) and with my own symbols. Designing symbols I take care only about having pins in 50 mils grid. As I prefer to have as small symbols as possible some symbols have for example pins on the right at x=100 mils and pins on the left at x=-50 mils. Even their center is not in 50 mils grid relative to their pins I have never noticed problem of positioning symbols.
Unfortunately I am now at PC (Win7) where I can’t install current KiCad version to do some experiments to check what I am writing.
The only problem with positioning off grid I noticed an year or more ago. I selected a small schematic block containing one symbol and few free texts positioned off grid. After moving that block symbol was positioned off grid. At the same time moving bigger blocks had no such effect. But since then I didn’t noticed such behavior - I’m luck or it was fixed in one of releases since then.
As people from time to time have problems with schematic off grid there is a function to reposition everything on grid, but I have never used it and having no KiCad at hand can’t tell where it is.
In KiCad it is quite important to work on a coarse grid, because netlist information is derived from coordinates of attachment points of wires and pins. If coordinates are off by even 1 mil, then KiCad does not recognize the connection.
KiCad’s default libraries are designed confirming to the KLC and all pins of all schematic symbols are on a 100mil grid. However, this grid does not always coincide with the origin of symbols.Especially very common symbols for resistors, capacitors and diodes are designed symmetrically around the origin of the symbol with a pitch of 300, and thus the pins are at a distance of 150 from the origin.
I have tried to work on a 100mil grid in the schematic for a while, but it is a big nuisance. You have to be constantly aware whether you grab a resistor by either a pin or it’s center when moving or copying it. If you switch the grid to 50 though, then all the nuisances disappear and it’s much more comfortable to design a schematic in KiCad. Working on a smaller grid then 50 does not have any advantage I can see, and it also makes alignment more difficult.
Because you maybe have yet to discover; there a couple of useful functions worth mentioning when dealing with schematic grids.
If you find schematic elements “off grid”, the easiest way to get get them back “on grid”, is to create a selection box around the entire schematic, right mouse click inside the selection box, then left click the “Align Elements to Grid” function. This moves all elements in that selection box on grid.
Holding the Ctrl key down, while moving anything, disables the grid. This can be useful when moving items, such as text (eg. Refs.) to more aesthetically suitable, but “off grid” locations.
mmmm. so what’s goign to happen when I import my Altium schematic libraries, thousands of them,
I’m used to working on a 100mil grid in Altium. The only time I might use a 25 or 50 mil grid is when I am makign a component in lib editor, and I want to put say, a sine wave symbol just between two pins, I’ll change to 50 ’ to do that, otherwise everything stays on 100mil. I’ll be interested to see durin gthe import whether kicad shrinks my 100 mil pin spacing down etc.
Kicad symbols are all based on 100 mil between pins as per the KLC mentioned above. The problem with using a 100 mil grid is when a symbol it held by its anchor (origin, centroid, geometric centre) instead of say, pin 1; and that symbol has an odd number in length eg. 300 mil. that symbol, when rotated, will have its pins land halfway between the grids.
See below:
By using a 50 mil grid, this assures all symbols will land on grid when rotated, whether the symbol is grabbed by its centroid or a pin.
