Separate NC Drill Files for Plated and Non-Plated Holes

[tarun172]

All,
     I was using advanced circuits (4pcb) for giving me a quote for a new design, I am currently working on. I noticed that you have option of having separate drill files for plated and non-plated files. I usually generate a combined NC Drill files for plated and non-plated holes. Why would you need separate files? Is there any advantage to using a separate drill files during manufacturing process (other than make it easier) or is it just a preference? I have heard some manufacturers say it makes it easier to manufacture but some say it doesn't really matter. I can see where things can possibly go wrong during plated/non-plated holes but I am still not buying on ease to manufacture thing here. Can experts shed some light on this issue? How does it make easier to manufacture?

- tarun172

[K5HJ]

The holes are drilled prior to the plating process.  Plating adds material in the hole so its size is reduced.
Randy

Edit:  I see you are talking about separate drill files for the same board.
That is unusual.

Never mind.

[xuio]

I always export seperate files. If you don't do this, how should they know which of the holes should not be plated?(apart from guessing based on copper connection and size)

Non-plated holes are drilled in the last step, often combined with routing.

Moritz

[mikeselectricstuff]

Not sure how common it is but my PCB SW (PCAD2006) annotates the drill file

M48
;FILE_FORMAT=2:4
INCH,TZ
;TYPE=PLATED
T01C0.016
T02C0.020
T03C0.035
T04C0.047
T05C0.071
T07C0.126
;TYPE=NON_PLATED
T06C0.118
%

[mrpackethead]

I always export seperate files. If you don't do this, how should they know which of the holes should not be plated?(apart from guessing based on copper connection and size)

Non-plated holes are drilled in the last step, often combined with routing.

Moritz

This is exactly why.

[Psi]

Yep, i always supply two NC drill files and name them to include the words plated and non-plated.

[forrestc]

I always export seperate files. If you don't do this, how should they know which of the holes should not be plated?(apart from guessing based on copper connection and size)

Non-plated holes are drilled in the last step, often combined with routing.

In theory, holes without an annular ring are non-plated.   At some (most? all?) board houses I've used, they drill all the holes up front then plate the entire board.   This results in *all the holes* being plated at this point.  However, in the etching step, the plating gets etched out of the non-plated holes since there is no etch resist over the non-plated holes.  Look at the copper layer in the gerbers for a board with plated and non-plated holes - the plated ones show copper over the hole, the non-plated ones don't - this layer creates the etch resist layer.   With no mask over the non-plated holes, the etchant can get into the holes and remove the previously plated copper.

That said, many board houses still want separate drill files.   But some don't.   Read the specs/file instructions for your particular board house before shipping off something wrong for that particular house.

[tarun172]

All, Thank guys. All this info really helps...
     

[marshallh]

With many fabs, they take 1 drill file, and whether the hole is plated or not depends on if said hole has any copper touching the hole.
No copper = unplated.

[Pjotr]

It is true that in one dril file, the plated and non-plated holes are clearly marked separately. However it is always wise to use 2 separate files for it and name them properly. I received from most fabs the non-plated marked holes still plated, even if there is no annular ring. They seem to ignore the non-plated marking in the drill file if they are in the same file as the plated ones.

[Psi]

I think the goal is to not make the pcb fab employee's job harder than it needs to be. They're not going to go out of their way to understand your files when you're paying $11 for 10 boards.

They want it as clear/simple as possible.