I ask this question because the smt plant of mine has reported an issue for me yesterday, they found an arc of edge cuts in gerber is different from mechanical drawing:
They want me to check which is correct. So I open the pcb in KiCAD, and click the arc to pop up properties bar, but I found there is only start x, start y, end x, end y, and arc angle。
There is no any data about diameter or radius.
So is there any way to check the diameter or radius for an arc?
On the bottom of your screen, under the work space, in the middle, is dx & dy.
Second button from the top on the left hand side is Cartesian/Polar switch button for dx&dy (amongst other things it does).
Clicking on the arc line shows the centre of the arc as well as other properties.
So,
Make dx & dy polar with the LH button (becomes R & Theta)
Click on the arc.
Place cursor on the now showing radius centre of the arc.
Press space bar to zero dx & dy.(R & Theta)
Move cursor to arc.
Read distance of radius from dx & dy (now called R & Theta)
That not how fabrication tolerance works. that ±0.05 either comes from the fabricators tolerance or the design tolerance w.r.t. the wider system once all the other parts stackup are aligned.
Worst-case the PCB is on the low-end of the radius and the mating shape is on the high-end of the radius tolerance. If we were to entertain what you are advocating, the GERBERS could ship with a radius of 24.4201. This HOWEVER means that whatever aligns with that arc has to then have tighter tolerance
GERBER at 25.46 (nom) and HOUSING at 25.36 (nom) which means if GERBER on the low side and HOUSING on the high side we would have 25.41 (assuming HOUSING tolerance is also 0.05). The GERBER is therefore taking up 80% of the “tolerance” purely in the nomimal digital file, which means the build tolerance of the PCB would have to be tighter than 0.05 (ie 0.01) to stay in spec OR the tolerance of the HOUSING would have to be improve (by 0.04)
In short, the digital formats should align to the agreed decimal place and the tolerance is the fabrication capability and what is required for full build
KiCad lacks this kind of sophisticated drawing capability, namely to translate the technical drawing seen above to line graphics in the PCB design. You have to do quite much mental work and even then the arc is defined by start, end and midpoints, so you can’t for example set the midpoint and the radius exactly as in the drawing. Something is lost in the conversion.
If it too close and no good they should make the tolerance tighter so the dimension shown is then actually out of tolerance . . . if it’s in tolerance its good enough.
I only said that it may be difficult in KiCad to draw with exactness something which may look easy in technical drawings. It wasn’t an answer but a comment. The direct question itself was already answered. If the original poster has difficulties with that specific detail, it may be better to try importing from some 2D CAD.
No, the tolerances of the housing don’t come into the calculation at all! That mechanical drawing shows the tolerance for the PCB, and the PCB alone: it already takes into account the tolerances of the housing, mounting points etc.
The bigger issue is whether the PCB manufacturing tolerances (on top of the design 's lack of accuracy) takes the arc beyond the specified limits. (the other thing that’s relevant, of course, is the position / accuracy of the “hole’s” centre point).
In reality, the given tolerance is probably not well thought out: if the “hole” is smaller, then you have an issue, but I suspect of the “hole” is larger, it’s not a big deal… you just have a bit of extra space… in which case it really could have been specified as “25.46 -.05 / +.1”
I do not agree with this.
Those tolerances apply to the physical product, and when you already eat up most of the tolerance by allowing faulty numbers in the CAD data, you increase the chance of problems during production, because the production process has inherent tolerances too. Allowing those numbers is sloppy work with a potential to cost a lot of money.
(Edit: I see now Naib also already mentioned this)
Don’t be ashamed. I checked your screenshot before posting my own screenshot. If your screenshot contained that data, I would have reposted your screenshot with the additional red arrow.
But it does make me wonder why that area does not contain the arc data on your screenshot.
Actually it does. That arc exists for a reason otherwise the PCB would be straight at that point. It is reasonable to assume that the arc in question is to fit around some other piece of hardware (eg HOUSING).
The entire mechanical tolerance stackup will account for all the tolerances
the PCB arc ( ± 0.05 )
the housing arc ( ± TBD )
All these tolerances would have previously be accounted for and thus the GA drawing should capture this. I am refuting that the electronic drawing and the GERBER are in spec as the discrepancy in the digital drawing and the GERBER are within the 0.05 tolerance (go back and see who I was replying to and their statement). This is not how that works. The GERBER and the GA should be exact to the agreed significant figure and then the tolerance of the PCB fabrication and the HOUSING fabrication should then be available for the fabrication of the respective parts and assuming they are within the tolerance they will mate.
kicad does not understand gerberas as a set of coordinates, it converts them into a picture for artists, this is the main difference from 2D editors… there is no way to work directly with the format
