Hey my follow Kicadets!
I’ve been using Kicad for roughly a month and I really love it.
long story short, I’m faced with some small challenges where the size and precise measurement of the pcb board matters.
here is an example with an image.
So I have made a rectangular drawing which is intended to be my pcb board and I used the “Draw a rectangle” feature to do it. the measurement is x-axis = 77.0600, y-axis 32.8400mm
which is pretty close to the exact measurement preferred.
this is the measurement I wanted :
77.0720 mm
32.8980 mm
but moving the mouse around can’t seem to fall accurately on these measurements,
thus I was wondering if there was a way of actually manually typing in the exact measurement
preferred or say typing in 32.900 and 77.070 without having to approximate it by moving the mouse around ?
Also, say I wanted to place the 2x20 connector header component right into the center of the
rectangle pcb or place the component at the far right end 10mm distance close to the edge of the board how do I achieve this ??
Thanks for you help
Kind regards,
Kevin
If you select a line, and then press e to edit it’s properties, you get a dialog in which you can directly enter coordinates:
This is a relatively complex aligment for KiCad, because it probably does not fit on any (normal) grid. But you can do it in two steps: First use PCB Editor / View / Grid Properties and set the origin of your grid to where you want to place something. Then grab your footprint by the right feature, and snap that to the grid origin.
Have you set the grid origin? There is a press-and-hold tool on the right and you can also get it from the Place menu. There is also a drill origin. Generally the drill origin goes in the lower-left corner of the board or array, and the excellon drill hits reference that. The Grid origin is for editing and can be in the same place as the drill origin, or if you have a special shape like a circle you may want the grid origin in the center of the board.
Also, the board edge is a closed path on the EdgeCuts layer. Eg: set the grid to your desired unit and size, put a rectangle on the edge cuts and drag it to size (or close), select it then press E to edit… Put the drill origin in the lower left of the board outline and grid origin as desired. Then start populating inside the board boundary (or building fragments outside and dragging it in when ready).
This means change the layer to “Edge Cuts” in the Appearance Manager to draw your board outline.
A useful feature is the “dx & dy” at the very bottom and middle of your screen (below your work area).
In the example case below I wanted to place the corner of the courtyard 150 mil down and 100 mil in from the board corner.
First select Positioning Tools > Move with Reference then click on the exact place you wish to position, the corner of the courtyard.
Next, move the whole symbol that is now attached to the cursor up to the board corner.
Next, press the space bar which will zero the “dx & dy”.
Next, move the footprint that is still attached to the cursor while watching the dx & dy.
When dx & dy show the correct value, press enter.
Note: for accuracy, zoom to a high magnification, use a fine grid and keyboard arrow keys.
You can also get the exact same result by using the “Move Exactly” or “Relative To”
For “Move Exactly”, place the courtyard corner over the board corner and then select Move Exactly.
Type into the now open box, X = -100 and Y = 150
Press enter.
Also, who will be cutting your board? What tool is being used to cut out your PCB, and what is its diameter? Is it a 1mm or 2mm contour router? Where is the measurement taken? Is it from the centre of the edge_cut line or from the edge and how thick is this line? You need to allow for these in your calculation of your PCB dimensions. It would be better to make it SLIGHTLY bigger so that you can trim it manually if needed.
paulvdh, teletypeguy and jmk,
A lot thanks for the instructions
the move with reference did the trick! However,
the line segment properties doesn’t make sense to me.
I’ll be honest that prior to asking for help in the forum,
I have already tried using the LSP and just couldn’t figure it out as to what is was doing…
It has a start and end point for X and Y with start and end point having completely different values.
when I modify any of the values, the board either shrinks or disappears or I don’t know… takes on some other shape. So how does it work exactly ?
Using my previous measurement say:
77.07 mm - X
32.9 mm - Y
How do I use the LSP to get this rectangle with these approximate or precise measurement.
Precisely, what values need I insert into X start point and end point etc.
djsbriscoe,
Never thought it would matter ??
I’m not sure yet but my first Go To would be pcbways I guess
I was wondering what could be difficult about the start point and the end point of a line. Then I noticed you are doing it with a rectangle. But with a rectangle it is not very much more difficult, although the labels are not very intuitive. But it is not very difficult. There are two X coordinates, (Left and Right side) and two Y coordinates (Top and Bottom).
In KiCad, by default the origin is always in the upper left corner of the “paper” / drawing area, but the direction in which coordinates increment depends on: PCB Editor / Preferences / Settings / PCB Editor / Origins & Axes
With the numbers below you should have a rectangle with your requested size. Note that you can also enter (simple) formulas in KiCad’s entry boxes. So **-100 -32.84 will be evaluated by KiCad to -132.84.
KiCad’s “absolute” coordinates always start in the upper left corner of the paper, but when you define the “Drill origin”, then that is also used for on screen coordinates. If you do PCB Editor / Place / Drill/Place File Origin and then put it on a corner of your rectangle, you see directly it’s size, without the offsets from the paper origin.
