Guard Rings on SOIC-8 Op Amps

I have some Ultra Low Current OpAmps for pH probe circuits - output will got to Arduino Mega.

With an SOIC-8 package, I cannot seem to get a THIN trace to go between the pin pads without violating the design rules (spacing obviously too tight). On one side I can use an NC pin to obviate the problem, but on the other I cannot.

Does anyone have any advice for putting Op Amp guard rings onto the PCB with this kind of IC package?

Thank You


Thank you - I watched the Video a couple of times and picked up some great tips/tricks. The program is amazing IMO, I learn how to use the thing in a day without reading a thing about it - just experimenting. Great job to all who worked on it.

Unfortunately this doesn’t solve the guard ring problem. I can make it work using 5 mil traces (passes DRC) but from the drop-down box traces this thin are unsupported by the fab house.

Here is the idea with 5 mil traces - these do not carry any current, they block stray currents from the surface of the board from getting to the high impedance signal at the input of the Op Amp by being at the same potential (voltage) as the protected pin/trace.

Any thoughts?


The guard trace still needs to follow the constraints/limits imposed by the fab house. Minimum trace width and keep out distance are both included in that. If they support a smaller keepout distance (minimum distance between traces), you can change that in “Routing” menu, “Autorouter Settings”, and select “Custom”. The default value is 10mil. That “SAYS” Autorouter settings, but the keepout is also used by the design rules check for validation. Reducing that will should allow thicker traces to fit between the pin pads. Next option is to use a footprint with narrower pads (a customized part definition). That would also leave more room to fit the design rules limits. It is going to be trade offs. smaller pads, smaller keepout, or thinner trace. The sum of all of those sizes can not be larger than the physical space available for the pin spacing. For a one off custom part, you might get away with moving the 2 problem pads VERY slightly away from each other, to get a bit more room. Move too far, and the part will not make proper contact when trying to build/solder it to the board.

That all makes sense - thank you. I brought up the current carrying point because it isn’t a current density issue - essentially a manufacturability and solderability issue.

One “solution” I’ve read involves lifting the pin of the IC OFF the board - and sky-wiring it to the BNC connector. In the end this might be clunky but it might be easier.

I was hoping that somebody had a clever work-around, or an idea that might make it easy…

Thanks again.

Instead of sky-wiring all the way to the BNC connector, you might try sky-wiring just far enough to get away from the smd pads. After that, there should be room for the guard trace.

Well that is a good idea - essentially sky wire to a pad - using a driven guard (rest of connections not shown):

Thanks! I hate the Sky Wiring but this alternative is actually pretty good. Of course I will make the pad a bit bigger to make the soldering job easier.

TLDR. The point of the vid was to show how to make the DRC distance smaller, and I think most fab houses can do 0.006". Just check with them. So long as the gap between the IC pins is 0.018", it should make it.

Translating/expanding from @Old_Grey’s numbers, with 0.05 inch (center to center) pin spacing, 0.032in wide pin pads, there will be a 0.018in gap between the pads. With a centered 0.006in wide trace, there will be 0.006in gap on each side. Converting to mils, that will be 50, 32, 18, and 6. If you can narrow the pads by 3mil, the 6, 6, 6 can be increased to 7, 7, 7 (or 6, 9, 6).

1 Like

You guys are terrific thanks.

Ok, if I want to thin up the pads a tad, I have no idea how to do that.

Before asking you, I loaded an SOIC-8 IC, selected it an opened the part Editor.

I couldn’t see what to do.

Is there a video example of such an operation?


The vids cover basic svg drawing as well as making parts.

The referenced videos provide the low level how to do it details. That level of manipulation is not included in the existing part editor tool. The summary, is:

  • open the existing part in parts editor
  • save as a new part
  • export the part
  • unpack the exported fzpz file into the separate part definition (fzp) and svg files (unzip)
  • modify the pcb svg to have narrower pins (using what ever tool you want)
  • combine the fzp and svg back into an fzpz (zip)
  • delete the initial saved part from Fritzing
  • import the modified part
  • place the new part from the MINE bin instead of whatever you are using now. (you can use “delete minus” to remove the existing part, while keeping all of the wires that will need to connect to the new part)

At the resolution you need to work with, you will need to be very careful to get accurate position and sizes, or there will not be quite enough room when you are all done. Which might be harder than expected, depending just how precise the coordinate information in the original part was specified. It might be easier to generate the nice regular array of pads you want, then copy/paste it into the copper layer. How hard that is will again depend on just how the existing pcb image was created and saved. There are some tricks to manipulating svg images that I do not know if are in the referenced videos. I am not going to try to cover options for that here. Wait until you get far enough to know what the question is based on what you find in the first several steps. If you want to start down this path.

As a first cut at finding out more about the part, once you get it exported and unpacked, the FritzingCheckPart can be used to see what (obvious) things might cause problems.

The vids show the above method, but the quicker way is to -
FZ edit part
Goto PCB view
Then File/Show in folder
Copy the svg file and edit that drawing
Then back to FZ edit and File/Load image for view, and save.

It saves all that unpacking and file conflicts.
There should be a vid showing the quicker way, but if it doesn’t, my soon to be posted vid will have it.

Here is the vid

Thank you again -

OK I did what you explained. Everything seemed to work perfectly with one detail I cannot seem to understand - I loaded the SVG in “Method Draw SVG Editor” - a Web based editor - and moved the pads as we discussed (Slightly, just enough to yield a bit more clearance, but I can still solder it). Then, saved it with a new name, then saw the new part show up in My Parts! Perfecto so far. But when I pulled the drawing in, the SCALE of the drawing was drastically different. The change I made was there, but for some reason the basic physical dimensions were drastically smaller.

Kind of fun - because the pad squeez worked like a champ, but something happened with the scale. All I did was pull up the svg, move the pad, and file it with a new name. How did the Scale get stomped on?

Maybe this is the attribute of the web based SVG editor?


Here is a zip file, renamed to .fzpz, with a slightly cleanup up version of the sparkfun analogic so08 pcb svg image, adjusted to use 1000 px per inch (1 mil per px). This uses 24 mil pad widths. Also in the zip file are modified versions with 21 and 18 mil pad widths. The forum would not let me upload the individual images. They are too small for it to figure out the dimensions, then the forum does not like zip files either, so renamed it to .fzpz

so08-footprints.fzpz (1.7 KB)

Here is a table of what maximum trace sizes will fit between the pins, based on the pad with and keepout distance. All numbers in mils

Spacing Pad Width Gap Keepout Trace Width
50 24 26 6 14
50 24 26 7 12
50 24 26 8 10
50 24 26 9 8
50 24 26 10 6
50 21 29 6 17
50 21 29 7 15
50 21 29 8 13
50 21 29 9 11
50 21 29 10 9
50 18 32 6 20
50 18 32 7 18
50 18 32 8 16
50 18 32 9 14
50 18 32 10 12

Smaller pads have there own down sides. For starters, to leave room for the trace between pads, the trace connecting to the pad can not be larger than the pad width. Another alternative would be a further customized footprint, with only specific pads being narrower, instead of all of them.

If fabrication handles it, I would consider the standard 24 mil pad size, with 10 or 12 mil guard trace

Thanks - it will take me awhile to work through this but I will - very much appreciate your efforts here. If you live close I will share wine from my winery if you like… :grinning:

OK - unzipped, pulled in the 21 mil version - edited the Metadata a bit, saved the new part - WORKS GREAT!!


:clap: :clap: :clap:

No modifications to keep out or anything - NICE!


Not much in the way of wineries near hear, so probable not close. Calgary, Alberta, Canada. But its a nice thought :slight_smile: