Precision coordinates

[alfalfa4381]

I am brand new to KiCad. I am reverse engineering a small pcb that has a geared motor that interfaces with a speedometer cluster. I want to lay out the pcb design in close tolerences, I want to enter the x-y coordinates in .001 inches Ie, the board is 2.370" x 2.480" and it is not rectangular in that it has angles and notches. I am used to a CAD where I can manually enter x-y coordinates. Can I do this in KiCad? If not, how would you do this? Thanks for your help!

[paulvdh]

You can not enter numbers during entry of objects, but once you have put an object (footprint, copper track, graphical item, etc) on the PCB, you can edit it’s properties and enter coordinates.

Whenever the mouse cursor is over the canvas, you also see the current coordinates in the status area at the bottom of the screen, and you can use the cursor keys to move the cursor over grid points.

Also, what sort of info do you have available of your geared motor?

if you have gerber files available, then the topic below is interesting:

Reverse engineering KiCad project from Gerber files

The goal of this reverse-engineering tutorial is to re-create a complete KiCad project from partial information assuming the only information available is a schematic in some readable, (but not EDA form, such as a .pdf or a .png picture), and a set of gerber files. The Gerber files will create a PCB with much PCB information missing, however, using this method is easier than re-designing a PCB from scratch, and can also be extended to any other program that creates Gerber files. What is “resc…

You can also use: PCB Editor / Place / Add Reference Image. With this you can import some nice photographs of real hardware to draw the PCB over it. It is recommended to have decent quality photographs, and possibly do some pre-processing such as barrel and perspective correction, maybe contrast enhancement and such.

But also: Don’t be too neat. There is no electrical need to reproduce the old thing as exact as possible, unless you want to make counterfeit products. Often it’s much easier (and quicker) to make it “sort of” the same and it is even likely you can do some optimizations to improve the layout to make it better then the original.

[jmk]

@alfalfa4381

I want to enter the x-y coordinates in .001 inches Ie, the board is 2.370" x 2.480" and it is not rectangular in that it has angles and notches. I am used to a CAD where I can manually enter x-y coordinates. Can I do this in KiCad?

No. As Paul says place first then move.

@alfalfa4381

If not, how would you do this?

As you are brand new to Kicad :
First open Preferences > PCB Editor > Origins & Axes. Set your X & Y co-ords. direction you are happy with.
Next: Set an appropriate Grid (red arrows)

It is possibly easier to create a complicated shape by starting with a rectangle.
Two easy methods:
Place a Grid Origin (green arrows), start a line on that origin and read the movement on X & Y (blue rectangle).
Similarly, pressing the Space Bar will zero dx & dy to the cursor position at that time, and movement can be followed with (yellow rectangle)

(cyan arrow) toggles between Cartesian and Polar co-ordinates. Good for angled lines.
(magenta arrow) restricts drawing angles. Good for straight lines and boxes.

Line lengths and widths can be changed in (Right Mouse Button) Properties. Lines can be moved (M) and dragged (G), but not broken.

There are also exact Positioning Tools for lines and footprints (RMB Select > Positioning Tools). These are self explanatory but need a few minutes practice.