I had my first PCB manufactured (by a Chinese manufacturer). In this first version I only used thru-hole components (not SMD).

I used the latest version of Eagle to design it, without taking care to set the pad (I hope is the correct name) dimension and shape. The program "decided" to use only circular pad around the component's holes for all the components.

Is the size of these pads (the dimension of the copper around the hole) in your opinion correct or it should be a bit larger (from what it is possible to see in the pictures attached)?

I noticed that soldering some components, the solder has not immediately spread on the pad, maybe because they are a bit thin.

I also don't know why sometimes the shape of the copper is oval and not circular in some circuit I have (not designed by me).

I attached pictures of the top and bottom of a zone in my PCB.

enter image description here

enter image description here

EDIT 1: with your help I would like to understand in which passage something went wrong. Eventually I can write an email to the manufacturer to understand better on their side. I opened the gerber file with gerbv and only switched on the files in the order TXT (drill), GBS and GBL. I attached 2 images with a focus in the second to capture the size of the anular ring (the gerber image corresponds more or less to the first real image but rotated). It is in your opinion the same dimension as in the real picture?

enter image description here

enter image description here

  • \$\begingroup\$ Take a look at the gerber files generated by Eagle, to double-check that it was Eagle that generated those pads. \$\endgroup\$
    – TimWescott
    Commented Jul 25, 2019 at 22:09
  • 3
    \$\begingroup\$ FYI the technical term for those copper donuts is “annular ring”, outer diameter and drill diameter. How much larger the annular ring needs to be, depends on the assembly process. For through hole, hand assembly, the pads need to be large enough that the soldering iron tip can contact both the pin and the pad at the same time. For wave solder or IR reflow the rules may be different. \$\endgroup\$
    – MarkU
    Commented Jul 25, 2019 at 22:18
  • \$\begingroup\$ your pads are all the same size as the tracks they are in. There is some mistake in your settings. The pads should be same size and not change depending on track. You should have checked before sending file. I use kicad, so don't know how to do in eagle. \$\endgroup\$
    – Indraneel
    Commented Jul 25, 2019 at 23:50
  • \$\begingroup\$ I edited my post with some gerber image. \$\endgroup\$
    – daigs
    Commented Jul 26, 2019 at 23:59
  • 1
    \$\begingroup\$ As the annular ring is minimal in your eagle screenshot, this looks like a design mistake resulting from not yet being familiar with what works well - fortunately, you can probably still use these, but design something better next time. Consider looking at designs for well thought out through-hole hobby projects, for example maybe some of the Adafruit or Sparkfun boards. Soon you'll probably end up developing your own library of basics tuned to your own preference. Also look into surface mount, it has so many advantages. \$\endgroup\$ Commented Jul 27, 2019 at 16:10

4 Answers 4


The exposed copper around a through hole is called the annular ring. The annular ring should be appropriately large to accommodate solder-to-pin wetting.

Your PCB fabricator should specify a minimum annular ring size, so be sure to check that. For example, OSH Park specifies 0.127mm (5 mil). Otherwise, when you design your PCB, you can generally add 0.25 to 0.30 mm (10 to 12 mil) to the hole diameter. (There are IPC standards such as IPC-7251 which you can follow if you need/want to.)

Conditions where you may want to increase the annular ring size:

  • Component needs physical strength, such as a connector or bulky heatsink
  • Component requires a large amount of current
  • Component will be soldered by hand or some other less-precise operation

Annular ring size decrease or modification would be due to:

  • Pitch or proximity of other pins on the component. Often oval pads are used when extra surface area is needed, but other pins are too close to allow a circular shape.
  • Other considerations such as solder bridges (depending on process)

For more information, see: How to determine annular ring width for thru-hole pads?

  • 2
    \$\begingroup\$ +1. Clarifying/adding, not disagreeing: The PCB fab house specifies the minimum annular ring that they can reliably manufacture without too much risk of the drill breaking through the ring. But that tells you nothing about whether it will be too small to comfortably / reliably solder - generally you'll want it to be considerably wider. \$\endgroup\$ Commented Jul 26, 2019 at 23:42
  • Yes, those pads look usable -- but barely.
  • Yes, they should be bigger.
  • Pad size and shape are determined by the footprint that the layout tool uses. Generally you choose the footprint.

On a completely different note -- those pads look much smaller than what is found in the Eagle library. I suspect that something happened between your Gerbers and the fab. Either the fab couldn't read your aperture files, or you misnamed them. Consequently, the fab applied their own defaults to how much copper should go around a hole.

  • \$\begingroup\$ Viewing the gerbers since added to the question, or even the picture of the original eagle PCB view, while the annular ring may have shrunk a little, it seems to have been rather marginal to begin with, more like the proportions expected of a via than those of a pad. Likely this was a design issue, not a manufacturing one. \$\endgroup\$ Commented Jul 27, 2019 at 16:06
  • \$\begingroup\$ Chris, sorry for the delay, could you explain a bit in depth? I'm not native english. It seems that the holes have "ate" a bit of anular ring during the drilling process, reducing it than what expected in the gerber. Do you agree? \$\endgroup\$
    – daigs
    Commented Oct 17, 2019 at 10:26

When you create a PCB layout you first need to obtain the manufacturer's design rules from the intended manufacturer of the board. Most PCB houses will supply their design rules in Eagle format so it is a simple matter to import them into Eagle.

If you want to have someone else assemble your boards then you also need to obtain the design rules, if any, for the assembler.

  • \$\begingroup\$ This is probably more a case of an inexperienced designer just not having an experienced eye for what makes a good pad. The fact that it is through-hole suggest there won't be an assembly service involved, yes, there are places that still do that but typically ones that refactor your design into what they think they can put together at the lowest cost. \$\endgroup\$ Commented Jul 27, 2019 at 16:08

For a plated through hole, the size of the minimum land (pad diameter) is specified by IPC-2221 "Generic Standard on Printed Board Design" in Section 9.1.1:

$$\text{Land size, minimum} = a + 2 \times b + c$$


  • a is the maximum diameter of the finished hole
  • b is the minimum annular ring (Table 9-2)
  • c is the standard fabrication allowance (Table 9-1)

The tables give you the parameters as a function of producibility level (defined in Section 1.6.3), copper weights, what to do for more than eight layers, .... For a simple board, the short version is: $$\text{Land size} = \text{maximum hole diameter + 0.7 mm (Producibility level A)}$$ $$\text{Land size} = \text{maximum hole diameter + 0.6 mm (Producibility level B)}$$ $$\text{Land size} = \text{maximum hole diameter + 0.5 mm (Producibility level C)}$$

Level A is the easiest to solder by hand. C is the hardest to do by hand.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.