Solder mask openings with multiple segments DFM Error

Layout
1

I am making a simple breakout board in Kicad-9.I will be soldering wires in the pad for measurements.The Pad footprint is taken from Kicad default library.The pad image is given below.

image
image2031Ă—329 47.5 KB

I generated the Gerber and uploaded to JLPCB DFM and I got the below error.

image
image1184Ă—968 68.4 KB

May I know how to solve this issue

2

Look at the Gerbers on the JLCPCB site and if it’s what you wanted you are good to go . . . their DFM is helpful but can be misleading/confusing.

While I’m here . . . why do you need such tiny skinny tracks ?

1 Like
3

This is a simple board conatins 4 of these sensors. It won’t take much current so I kept trace width as 0.2mm.
May I know any issue with 0.2mm width

4

They are fragile, you are asking JLCPCB to remove more copper, you are paying for the copper don’t you want to keep it ? a thicker trace adds strength to where it joins the pad, there are many reasons . . .

1 Like
5

Thank you I will increase it.
May I know is there any method such that I can change the width of all tracks in one shot

6

Select them all, right click, properties then if you have the Property manager visible you can set all the widths at the same time.

1 Like
7

Thanks a lot.

I changed the widths to 0.4mm

For some pads it is coming as shown below.I hope that is fine.
Could you please confirm

image
image526Ă—622 14.7 KB

8

For thin tracks, there are a few disadvantages.

  1. They do become more fragile, Sensible for scratches, and the chance of them developing hair cracks right at the end of the pads is real. Using teardrops eliminates this because the gradual width change reduces mechanical stress (especially with stiff THT connectors).
  2. It’s not always compatible with the cheap 2-layer proto service. 0.2mm is around the minimum width for some of the 2 layer PCB fabs. Exact limites are not a hard cliff, but if the tracks are too narrow for the machines used, it’s more likely to have etching faults. Multi-layer PCB’s (4 or more layers) are generally made on a higher resolution production line and 200um tracks are no problem at all.
  3. Thin tracks do have more copper resistance, and therefore a higher voltage drop. But a 0.2mm track can still handle 750mA. In that case temperature rise is 10c, resistance for a 100mm track is 0.24 Ohm and voltage drop is 182mV. Most signals on a PCB are below 20mA (so 60x smaller) and this is not a problem. But you have to be aware of it.

Wider tracks also have disadvantages.

  1. They have more capacitance, especially with high speed digital signals on multi layer PCB’s (with only a thin prepreg between signals and GND) this can be important.
  2. They take up more board space.

Shorting pads in this way is no problem at all for the electrical connection, but it does make inspection more difficult. Especially when the pitch is fine, there is no room for solder mask fingers in between the pads. As a result, a solder blob will form between two of such pins. And when you do a visual inspection, the first thing you do is wonder whether that solder blob is a fault or not, some people may try to remove it without even checking documentation. But most would have a look at the documentation. When the “short” is routed as a bow around the pads, then visual inspection is a bit easier.

2 Likes