Creating a NPTH requires proper soldermask expansion and copper pullback from the edge of the hole.
3D Color View
If the design calls for a NPTH as show above (P2) a circle arc can be used to create the ring around the un-plated hole.
Note that the soldermask was not pulled back from the edge of the hole for P1.
The designer of this NPTH will get a technical query from the PCB fabricator asking for permission to pull back the soldermask from the edge of the hole.
Shown in 2D the soldermask is correctly pulled back from the edge of the hole for P2.
Are we done Now ?
.
.
.
.
.
Before answering that question, let's look at typical surface mount pad.
Note soldermask expansion, which is typically 4 mils.
The soldermask registration accuracy needs to be considered.
More work is needed to properly finish this NPTH.
Let's add a 5mil expansion to the arc (full circle)
Ok, now we are done. P2 is good to go.
There may be other factors to consider, like copper pours with same or different net than the ring around the hole.
That's It !
When creating a Non-Plated Hole such as a Tooling Hole if you forget to uncheck the Plated option you will most likely get a technical inquiry from your fabricator.
I wish there was a design rule check under the Manufacturing Rules to catch this mistake.
As shown below the pad and hole are set to the same size to create a NPTH. However the user forgot to uncheck the plated option.
To find a NPTH that is incorrectly checked as Plated you can use this PCB Filter:
(PadIsPlated = 'True') And ((HoleDiameter >= PadXSize_AllLayers ) OR (HoleDiameter >= PadYSize_AllLayers))
Copper Clearance Rule (Standard is 10mil)
Plane Clearance Rule
For Non Plated Holes (if Plated is unchecked) you can use:
(HoleDiameter > 0) And (PadIsPlated = 'False')
For both Plated or Non Plated Holes use:
((HoleDiameter >= PadXSize_AllLayers ) OR (HoleDiameter >= PadYSize_AllLayers))
Soldermask Expansion (Standard is 5mil from Hole Edge)
If the Soldermask and Copper clearances are both 10mil. The 10mil copper clearance is good for the internal layers, but what about the outer layers ?
To prevent having a NPTH with exposed metal on the outer layers you need to consider the layer registration tolerances.
That's It !
Design for Manufacturability (DFM) for Non Plated Thru Hole (NPTH) the soldermask opening should be finished hole size (FHS) + 10mils.
Example: NPTH for test fixture tooling, soldermask = FHS + 10mil (0.25mm)
In Altium this means the Soldermask expansion should be +5mils (0.125mm).
You should also include a copper keep out on all layers of FHS + 10mils.
There are no Design rules or DRCs in Altium for Non-Plated Thru Holes that will catch this DFM issue.
