plated and non-plated holes

I have both plated-through and non-plated holes on many

of my PCB designs, and so do many, many other people.

Plated-through holes are used for vias and component leads.

Non-plated holes are used for component mounting or attaching

the PCB to a chassis via mounting hardware like screws.

All plated-through holes should have an annular ring around

them on both sides of the board. Non-plated holes have no

annular ring and no metal in the hole barrel and are thus better

suited to threaded hardware than plated-through holes are

because the possiblity of metal shavings coming off during

insertion and removal of hardware is eliminated.

Does your PCB service support both plated and non-plated

holes? I know the board shop does, but does your “BOT”?

Industry standard practice is to submit two drill files with

a PCB data package. I use the following standardized names

for these files:

drill_plated.drl # plated-through holes, Excellon format

drill_nonplated.drl # non-plated holes, Excellon format

If you don’t allow two drill files per PCB, you should add this

capability, and update your FAQ on board submission accordingly.

I’ve made several PCB’s with large commercial boardhouses - with plated and non-plated holes - and I have never submitted two separate drill files, nor have they requested them that way. I’m not sure what industry standard practice you’re referring to…

–David Carne

busonerd:
I’ve made several PCB’s with large commercial boardhouses - with plated and non-plated holes - and I have never submitted two separate drill files, nor have they requested them that way. I’m not sure what industry standard practice you’re referring to…

–David Carne

How did the board shop(s) distinguish between the plated

and non-plated holes? If you sent them a drill drawing

(the traditional, now-obsolete way), then they used their

CAM system to generate two different drill files from your

data. Why? Because most board shops drill the plated holes

first, then plate through the panel, and just before the boards

are routed out, the non-plated holes are drilled. There are

many steps between drilling the plated and non-plated holes.

The industry-standard two-file submission I spoke of is for

direct use by the board shop with NO other processing required

on their part, other than possibly shifting (translating) and/or

stepping & repeating (arraying) the files.

I sent them the plain drl file - I assume they just plated based on whether the hole had an annular ring ;).

–David Carne

I think the batchpcb service doesn’t offer non-plated holes, but I can’t find a pice of text saying so right now.

All holes are plated. Non-plated holes take an extra handling process. We do not offer non-plated holes.

-Nathan

sparky:
All holes are plated. Non-plated holes take an extra handling process. We do not offer non-plated holes.

-Nathan

OK, no problem. This means that ALL holes should

have an annular ring on both sides. I recommend a pad

size at least 0.020" (20 mils) greater than the hole size

so that drill/pad misalignment (part of the manufacturing

process) does not cause annular ring “break-out”.

Gregben,

You’ll find most proto shops only offer plated holes, as it eliminates a 2nd drill step after processing.

I think you mean to propose that drill holes have a clearance from copper traces / planes. In Eagle, this is defined in DRC on the Clearance tab, and will hold back the copper planes from the drill holes so that drill misses don’t short the two planes after plating.

Size of the clearance depends on the accuracy of the drill. 10mil on each edge of the hole is usually enough.

(Sorry to be pedantic, but annular rings are the copper rings around the via hole. They aren’t needed for plain holes, regardless of plating.)

Cheers,

Richard

Richard:
Gregben,

You’ll find most proto shops only offer plated holes, as it eliminates a 2nd drill step after processing.

It depends on the level of sophistication of the proto shop. The ones I supply tooling and film to offer both plated and non-plated holes along with routed internal shapes.

Richard:
I think you mean to propose that drill holes have a clearance from copper traces / planes. In Eagle, this is defined in DRC on the Clearance tab, and will hold back the copper planes from the drill holes so that drill misses don’t short the two planes after plating.

Size of the clearance depends on the accuracy of the drill. 10mil on each edge of the hole is usually enough.

(Sorry to be pedantic, but annular rings are the copper rings around the via hole. They aren’t needed for plain holes, regardless of plating.)

Cheers,

Richard

No, I mean that every hole should have a metallized ring around it.

This is because in most board shops, the photoresist “tents” the holes during the etching step (at least for panel-plated boards). If the tent doesn’t extend past the edge of the hole it can cause etchant leakage into the hole. This may in turn cause loosening or destruction of metallized barrel in the hole that was formed during plating.

This makes it a good idea to provide an annular ring around ALL plated through holes whether vias or not. Annular rings are also essential around any hole that has a trace leading to it. Vias and component mounting holes fall into this category.

It seems strange to me that GP offers custom routing and board dimensions (with any wierd, rounded corners and non-standard edges you can think of), but not unplated drilling. I know next-to-nothing about the process, but it seems logical that this should be an extension of the custom-routing capabilities.

Learn something new every day, I guess…:slight_smile:

roach:
It seems strange to me that GP offers custom routing and board dimensions (with any wierd, rounded corners and non-standard edges you can think of), but not unplated drilling. I know next-to-nothing about the process, but it seems logical that this should be an extension of the custom-routing capabilities.

I’m just taking an educated guess here:

They don’t offer non-plated holes because the routing machine they

use is designed exclusively for routing (has a routing spindle) and

does not have drilling capability. To offer non-plated holes they

would have to run the panel back through the drilling room/area

then on to the routing room/area. They could do it, but it does take

some effort to setup and costs money to do because of the extra

steps/labor.

In the shops where the router has a combo drill/route head and

automatic toolchanger it is easy to do non-plated hole drilling

followed by routing in one setup.

I’ll put in my two cents here:

I don’t know the fab process well enough to say. I faintly remember reading that the holes had to be filled with a substance to prevent the plating. So it may not be as easy as a second drill process.

Who really needs non-plated holes anyway? We’ve done lots of protos and designs and never had the need. Just stick a hole there!

If it’s not a via, why put an annular ring around it? That’s silly and wastes space. Make your annular ring 0. The stand-offs don’t care if there’s copper there :slight_smile:

-Nathan

sparky:
I don’t know the fab process well enough to say. I faintly remember reading that the holes had to be filled with a substance to prevent the plating. So it may not be as easy as a second drill process.

One method to create non-plated holes is to plug them (usually with little rubber corks) before plating. This is an old technique though, and I don’t think many

manufacturers use it any more.

sparky:
Who really needs non-plated holes anyway? We’ve done lots of protos and designs and never had the need. Just stick a hole there!

Protos don’t matter much – but if you ever want to go into production it is handy

to know how to do this stuff properly.

sparky:
If it’s not a via, why put an annular ring around it? That’s silly and wastes space. Make your annular ring 0. The stand-offs don’t care if there’s copper there :slight_smile:

-Nathan

Well, let’s see. I’ve been in the PCB business since 1988, and…

If you want to bond to ground then you need an annular ring, and of course the screw head takes up lots of space, so you certainly aren’t going to

waste space by putting an annular ring around screw holes. If you use plastic

snap-in standoffs there still isn’t any harm in having a 20 mil ring of foil around

the hole. It might be interesting to ask your board shop what they think.

One method to create non-plated holes is to plug them (usually with little rubber corks) before plating. This is an old technique though, and I don’t think many manufacturers use it any more.

Hi gregben,

I’ll add a few thoughts to what you’ve written about manufacturing processes.

First of all, a lot of routers can drill too. All of them should be able to, since they’re basically just drilling machines with spindles designed to be be dragged sideways through panels.

As for unplated holes, if the PCB shop uses the procedure I’m familiar with, then tenting will result in a non plated hole. That is, if you don’t put pads on a hole, and there’s no other copper around the hole, the result will be that the hole will be unplated.

There are three ways to produce an unplated hole.

One is post drilling, one is plugging (this is extremely tedious and error prone) and the third way is tenting.

I’ll try to explain how tenting works. The manufacturing procedure is first to drill the panel, then to use electroless copper plating, or direct metalisation, or some other way to get a very thin layer (a few microns) of copper in to the hole barrels.

Next dry film photoresist is applied to the panels, and the film with the track image is lined up with the drill holes and the photoresist is exposed to UV light through the film. Then the panel goes through a developer which strips off all the unexposed dry film. The result is that the panel now has plastic film stuck to it everywhere where there’ll be NO copper on the final board. (This means that holes with no copper pads will be ‘tented’ by the film top and bottom.)

The next stage is electroplating copper. The factory where I work plates close to 1 ounce thickness of copper, so the holes will get about 1oz copper thickness and the top and bottom copper will be close to 1.5 oz since we start with 0.5 oz material.

After copper plating, tin/lead is electroplated as etch resist.

Now the dry film is stripped from the panel. The panel now has plated copper covered with a tin/lead layer whereever there’ll be copper on the final panel. The remainder of the board has thinner bare copper shown, not plated with tin/lead.

The next step is etching, which removes all the copper which does not have the tin/lead etch resist coating. This includes the few microns of copper that was inside those tented holes.

So… Provided that the manufacturer follows a procedure similar to this one, tenting holes by removing top and bottom copper pads will result in unplated holes.

I have two notes to add to this. First of all, if there’s any copper at all touching, or very close to the hole (on the design) including tracks, pads, or fills, then there’ll likely be some plating in the hole. This will also be the result if the tenting over the hole breaks or is washed off. This is more likely to happen with large holes, perhaps 4mm and larger.

The other point is that manufacturers increase the diameter of the holes by about .004" to allow for copper plating and solder coating. So if you choose the tenting method for acheiving unplated holes, your unplated holes are likely to come out slightly larger than you specified.

The advantage of using the tenting method is that you can do it yourself and not even bother to tell the manufacturer that you want unplated holes. Once again, of course, this assumes that they use the manufacturing process I’ve described above.

Another advantage is that the unplated holes, since they are drilled at the same stage as your component holes, will align with them better.

On the other had, the advantage of post drilling unplated holes is that they’ll align better with the routed edges of the board, if they’re done on a driller/router in one step.

By the way, the term ‘tenting’ is also used in relation to vias. If there’s no solder mask pad on a via then it will end up ‘tented’ with solder mask ink.

Steve.