Hello, I’m not very experienced in using kicad and have made maybe 1 or 2 pcbs using it at this time.
I am looking for a way to draw pcbs to exact dimensions and am having a very hard time figuring out how.
I am used to what other cad packages do where they let you add dimensions to a drawn item and it automatically adjusts to the dimension you type in (like shown this picture taken from fusion 360) (https://imgur.com/a/UgBCn7B)
Ideally I would like to draw my pcbs in the same way but it does not seem that kicad has an option for this, any input is greatly appreciated.
For simple shapes like that you can just set your grid spacing larger. You can also add measurements with the “add measurements” tool on the right tool bar. Them move it or delete it once done.
EDIT: Once you set the grid, right click on the pcb, you can watch the distance at the lower right of the window. Spacebar will reset to the current cursor position for easier reference.
Fusion is a parametric cad program. KiCad (and most other ecad programs) is a direct modeler more like autocad (But without draw command entry field so you really only have the grid. Measurment tools for checking the result exist in the inspect menu.)
There are plans to add some support for parametric paradigms but the earliest we can see something like this will be with v6 so in two years or so. And it remains to be seen which things will be parametric and to which degree.
If you want to work with parametric modeling software then you can do that. KiCad can import dxf so this option always exists (But be careful which dxf version you generate and which features you use. not everything is supported by kicad. For details about that search the forum as i have very little expirience with that.)
Your thread title is a little misleading. KiCAD CAN create a board outline specified to a greater precision than any manufacturer can deliver, as long as the outline is fairly simple. You simply specify the location of every line segment in the outline - a tolerably tedious process for rectilinear outlines with no more than, say, a few dozen segments. Same thing for parts placement - edit the component’s “Properties”, all the way down to nanometers if you’re that picky.
As a practical matter, when a board outline becomes much more complicated than a basic rectangle, I create it in the stand-alone drafting program “LibreCAD” and import the result to KiCAD as a *.DXF file.
When it comes to creating a classic drawing showing dimension values, etc, KiCAD can add the arrows, leader lines, numeric values, etc . . . . but . . . . they aren’t attached to any particular object.
The above image is a reasonably well-done drafting project, if I do say so myself. But even though each of the dimension call-outs is visually associated with some feature in the displayed image, in fact they are independent objects that just happen to be floating in space near a particular line, vertex, center point, etc. For all of the software sophistication and digital advances that have gone into KiCAD, when it comes to adding dimensions and notes I might as well be working with a T-square and drawing triangles on a hard-maple drafting table, like my father did over 80 years ago.
Do I wish KiCAD was more capable in this area? You bet! Is it likely to happen any time soon? Don’t bet on it! In fact, this whole style of presenting information seems to be fading away, perhaps analogous to the demise of beautiful calligraphy documents produced in monastic communities before the advent of printing presses. I have learned to look at such a document and take in both its broad scope and specific details by visually scanning it. My co-workers - at least, those who have the time to be bothered by drawings at all - would rather open the drawing on a display screen and clicky-clicky to get information about some item or feature that is relevant to the moment.
you can use kicad stepup (a freecad extension) to get your board into a good open source mechanical (parametric) cad program. You can then use the drawing dimensions or techdraw workbenches to derive a dimensioned drawing of your board.
Yes, it seems most PCB design programs lack sophisticated drawing tools. For complex board outlines I’ve always just drawn them in AutoCAD then exported to DXF then import the outline into CADSTAR or KiCad as needed. Then finish the board, export the DXF then pull that into AutoCAD to add all of the dimensions and other views. Makes a nice cross check of the original design. Although nowadays at least with CADSTAR I use their IDF interface to export the design to Solidworks so it can be used in my mech guy’s 3D model. As long as KiCad can do basic DXF import and export that should be good enough I think even for complex designs. The workflow for those involves mechanical 3D modelling so no need to reinvent the wheel on the part of the KiCad developers when it comes to drawing tools.
