Platform forum

How to create Guard Ring( i.e. NO solder-MASK and NO solder-PASTE upon a track?

Somnath123 , 01-11-2022, 11:07 PM
Hello Robert,
Really thanks for making such a detailed youtube video. It has helped me to get a deeper understanding of PCB design.

Actually, I am working on a GUARD RING concept and I want a pure copper track with "NO MASK and NO PASTE" on it. And there are no detailed videos available on the internet. I just found only one ( The video I refer to
), but It did not help me. It will be easier for students like us if you can make a video on the same topic.

I followed the same procedure that is taught in the above video... But after fabrication, solder paste remains on my track (Refer to attached Fig.1).

So I have to etch out the top-paste by myself (Refer to Fig. 2)
But it is very risky as it breaks while etching using Sharpe bleed.....How to achieve this while designing the PCB in Altium?

Thanking you in advance.
WhoKnewKnows , 01-12-2022, 05:02 AM
Why must it have no solder mask?
Somnath123 , 01-12-2022, 09:28 AM
When we deal with very high resistance (in my case 1GW) then PCB leakage current has a very high effect on a sensitive node (Inverting and Noninverting terminal of an Op-Amp). So, we must reduce the PCB leakage current. This is done using Guard Ring.
Guard rings surrounding critical signal traces, when properly applied, can significantly reduce PCB surface leakage currents into critical (high resistance) nodes. These guard rings have no solder mask and no solder paste, so that the leakage currents flow into them, instead of into the sensitive trace.
For more detail refer to this document

WhoKnewKnows , 01-12-2022, 11:29 AM
I understand the use of guard rings, or thought I did. I didn't realize they needed to have no masking. My understanding is that the leakages of concern are arriving to the sensitive circuits by traveling through the PCB substrate material. I imagine solder mask material has a higher dielectric constant than typical FR4, so keeping a guard trace open at the surface would mostly guard against surface currents, and those surface currents would most likely flow through surface contamination. (Side note, be sure to spec high level of cleaning, handling only with gloves, etc.) IE, if you keep the board clean, you shouldn't have to be concerned with the guard trace being exposed through the solder mask.

To get it exposed anyway, I would use a net tie at each end of the loop so that Altium treats the guard trace as a unique node, and layout normally. When layout is complete, go back and manual add openings to the solder mask over the guard trace. I wouldn't open the solder mask for the guard trace in places that make the PCBA difficult to manufacture, like where the guard trace passes under the chip resistors. Note to your fab shop that you want these areas to remain clear of contamination including surface treatment as is done with pads. Otherwise, it will get whatever surface treatment you select, HASL, ENIG, etc.

You may find you want something on the bare copper surface to prevent corrosion. Talk to your fab shop about it.
qdrives , 01-13-2022, 09:52 AM
A couple of additional remarks to add to @WhoKnewKnows
1) I think you mistake the paste mask with surface treatment (HASL, ENIG, etc.)
2) The application note only talks about solder mask, not the surface treatment.
3) To prevent paste and solder mask, you select the traces and arcs and set soldermask expansion to rule and set a (positive) value for solder mask expansion. Paste mask for tracks by default is not applied.
4) I have not read the application note extensively, but I do think a guard ring works better if the area is smaller.
WhoKnewKnows , 01-13-2022, 10:38 AM
There may be a compromise to consider. Perhaps by placing the guarded resistor nodes spaced away from each other, they are better isolated from each other's potential mutual leakages, but more exposed to surrounding leakages. Closer together and shorter guard trace may reduce external leakage exposure at the cost of mutual leakages exposure. Just thinking in terms of theory. I don't actually know for certain. Another strategy or additional strategy could allow use of slots in the PCB to help minimize leakage exposure along with location and guard trace. Good luck 🤞. And, let us know how it goes
WhoKnewKnows , 01-13-2022, 10:41 AM
Perhaps a guard trace should go down between the guarded nodes instead of simply surrounding them?
Somnath123 , 01-13-2022, 10:41 AM
Thank You @qdrives

3) Is there any specific number I should enter or any positive number will work?
4) even I also felt the same. But what do you think, Can I consider 2cm X 2cm as a smaller area? because that is the current size of my guard ring.
Somnath123 , 01-13-2022, 10:49 AM
Thanks, @WhoKnewKnows

But theory says the GR should be tied to a voltage equal to the Inverting and Noninverting terminal of OpAmp, So I tied it to the Vbias Potential (My Design is Single Supply) . . .But When you say "guard trace should go down " what do you mean?. . .Could you please explain it little more detail.
WhoKnewKnows, 01-13-2022, 11:19 AM
I was thinking perhaps each guarded node should be surrounded by its own guard trace instead of surrounding them all with a single trace. Just speculation
Somnath123 , 01-13-2022, 10:56 AM
and one more thing my earlier design has failed. But when I place this guard ring. . .My design has worked.

But In the current situation, I want the solder paste should not to be present after fabrication?
Somnath123 , 01-13-2022, 11:02 AM

I referred the document at Altium Website. . .It says to set a NEGATIVE VALUE for the solder mask expansion. . . Now, I am confused, What value should I key in?

Please help. you guys are more experienced than me, So whatever you say, I will do that.
robertferanec , 01-14-2022, 07:54 AM
Just go on solder layer and Place -> Fill - draw rectangles that areas will be unmasked. You can simply verify that in 3D model.

Somnath123, 01-14-2022, 09:06 AM
Thank You Very Much @robertferanecVery happy to see a reply from you. Just want to bring to your notice that, from my last fabrication-I did the same thing (steps you explained) and I got the expected results (there were openings- NO solder-MASK over it). But solder-PASTE WERE LEFT UPON THE TRACK.. .My concern is - "How to make sure that there is NO-PASTE upon the opened track".
robertferanec , 01-14-2022, 09:44 AM
as @qdrives mentioned, did you use ENIG PCB finish? If not, they will put "solder" everywhere during PCB manufacturing - but that is not the paste layer, that is PCB finish which will cover all unmasked area.
Somnath123, 01-14-2022, 10:37 AM
What is ENIG finished PCB?If I ask my fab-house, they will just do it or I need to do something while designing the PCB in Altium.
qdrives , 01-14-2022, 01:59 PM
Again, I think you mistake solder PASTE with solder MASK. Even though they may seem similar, they are, in fact, completely different (although it could be up to 90% inverted image.
Solder PASTE is used to solder the SMT components to the board using - solder paste.
The solder MASK is used to state where the 'copper' surface need to open, that is, not covered by the (green or your case blue) solder mask.
As I said in the first line, they may be 90% identical as a SMD pad both needs an opening (solder MASK) and PASTE to solder the component.
Solder MASK photo: https://external-content.duckduckgo....jpg&f=1&nofb=1
Solder PASTE photo: https://external-content.duckduckgo....jpg&f=1&nofb=1
Soldering process video: https://youtu.be/xqv9HF_2GlY

Another item is the surface finish. Two of the most used finishes are HASL (Hot Air Solder Leveling) and ENIG (Electroless Nickel Immersion Gold). HASL (or lead free HASL) is the cheapest. Looking at your photo, it looks like HASL. And yes, it may look as if the board has been solder - which is EXACTLY the case. A surface finish is required as bare copper is terrible with oxygen and the finishes are not. If you have not specified a specific finish, the fabricator will select one for you.
A video about HASL: https://youtu.be/IjsqukppWfw
Production step for PCB production: https://www.eurocircuits.com/Making-...-step-by-step/

The application note you mention only talks about keeping the solder mask from the guard ring "These guard rings have no solder mask..." (page 12). It state nothing about a surface finish or soldering.
So it should be OK.

Additional comments:
- New layout seems a lot smaller and in my expectation better.
- Do keep in mind that there is a minimum trace with.
- You can specify a solder mask region or something else on the solder mask layer like @robertferanec mentions. However, you can also set the solder mask for the traces and arc like in the picture below. With the method Robert does, it is either a more manual activity, or a large area no longer has solder mask as you uncover the entire area.

The result is here:

And you can play with the solder mask setting too, both positive and negative and like Robert said "You can simply verify that in 3D model." (well "view" not "model", but good enough)

- You mentioned "and one more thing my earlier design has failed. But when I place this guard ring. . .My design has worked." The guard ring should not be the difference between working and failing, but more reliable and accurate (less noise or drift).

- From what I know and it is also stated as bit the application note "The guard ring is biased at the same voltage as the sensitive node; it needs to be driven by a low impedance source." (page 12). In all the examples show the ring it attached to either inverting or non-inverting node AT THE OPAMP.

- Looking at the layout, and expecting schematic I think that a different layout will make a much greater improvement than the guard ring would. The output trace is long and goes around to both ends if the input circuit.
Somnath123, 01-18-2022, 07:05 AM
qdrives Really thanks for the extensive explanation. You were right... I misunderstood the solder PASTE with 'finished PCB' (In my case, the white color lead upon my PCB is HASL finished surface, confirmed by my fab-house)... Now I get a full understanding of all the above-mentioned points and theories.You were right the Guard Ring help in reducing the noise and drift, enhancing the stability of the system. GR only needs the opening (i.e. NO solder MASK over it) and I don't have to etch the finished PCB as it will be affected by oxygen and get corroded after a period of time. Point to be noted: 1. While designing the Guard Ring, It is important to provide a path for the leakage current and it should be properly biased depending upon a power (Single or Dual) supply configuration of OPAMP.2. The GR should be small in size (most people thinks the same)
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?