Drill to PAD Clearance

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
PaulNewf
Posts: 42
Joined: 20 Jan 2016, 08:33

Drill to PAD Clearance

#1 Post by PaulNewf » 27 Feb 2020, 16:03

I have "TopDown" LEDs that have a drill hole between the pads for the light to shine through.
The hole is of course very close to the pads, but is manufactured and assembled fine by PCB supplier.

but...

Every time I run Verification all the LEDs are flagged as errors with drills too close to pads.
There are many of these so they tend to blanket the DRC report, I'm trying to remove them so I can see real errors.

Error:
Pad L1:K - Drill (Gap=0.0571mm; Rule=0.2mm)
Pad L1:A - Drill (Gap=0.0571mm; Rule=0.2mm)

I've tried without success, the error always occurs: (Gap=0.0571mm; Rule=0.2mm)
- Tried: set the Pad-Drill clearance to 0.0mm (in Design Rules - Clearances)
- Tried: disable DRC for all Netclasses

I can't find which setting is controlling this drill-pad rule, any ideas?

Using DipTrace3.3.1.3

Any ideas?

Paul

PaulNewf
Posts: 42
Joined: 20 Jan 2016, 08:33

Re: Drill to PAD Clearance

#2 Post by PaulNewf » 09 Jun 2020, 08:18

Just trying to DipTrace4002 and I see same issue for TopDown LEDs and clearance between the centre drill hole and rest of footprint.
There appears to be many more clearance settings in DipTrace4002, but I can't seem to find where to adjust these clearances to remove the issues.

Any Ideas what I need to change to cure these items?
Pad L1:K - Drill (Gap=0.0571mm; Rule=0.2mm)

It would help if which "Rule" was more clear, many rules but no idea which clearance is actually violated.

Paul

Tomg
Expert
Posts: 1541
Joined: 20 Jun 2015, 14:39

Re: Drill to PAD Clearance

#3 Post by Tomg » 09 Jun 2020, 12:37

Who is the manufacturer and what is the part number of the LED being used? (Does it have through-hole or SMD pads?)
Are you using a pad for the light port or are you using a mounting hole?
It might help if you could post screen shots of the following...
* Your Design Rules dialog window (click on its [Clearance] tab).
* A closeup of one of the LEDs in the PCB Layout editor.
Tom

PaulNewf
Posts: 42
Joined: 20 Jan 2016, 08:33

Re: Drill to PAD Clearance

#4 Post by PaulNewf » 10 Jun 2020, 11:06

I created a minimal layout to show the issue and settings, and that seems to have given me a partial solution.

Wish Route-Netclasses Clearance Details offered Drill and Board Edge settings (Like Design Rules Clearance Table).
Wish Netclasses Clearance Details window indicated what it covered by the General Netclass Clearance setting.
- there aren't "drill" or "board edge" settings under "Netclass Clearance Details"
- the general "Netclass Clearance" setting does affect drill clearance (and possibly board edge clearance or something else?).

So solution for me at this timer is to set:
- Create a custom Netclass for signals connecting to these LEDs (not possible for LEDs directly connected to Power or Gnd signals).
- Netclass Clearance = 0.05mm
- Netclass Details = All = 0.2mm
- Design Rules Drill-SMD Clearance = 0.05mm (Drill-SMD already 0mm)
- Unsure what else is affected by two 0.05mm settings (Clearance of what other things?).

----- extra info -----
There are many "Top Down" "Reverse Mount" LEDs.
I tend to use these as the round lens is easier to make a hole for than the square lens.
- Dialight 597-6001-607F and 597-6501-607F

Attached file has my working footprint in a library, some images, and some links.
- TopDownLEDsV03PR.zip

Paul
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1541
Joined: 20 Jun 2015, 14:39

Re: Drill to PAD Clearance

#5 Post by Tomg » 10 Jun 2020, 16:00

Other than hoping the DipTrace developers add a "[x]Suppress Error" option to each line of the DRC report some day (I would like to see that), you might consider customizing the pattern to just barely pass the current rules. In the example below (units = mm), pad size has been changed to 1.44W x 1.59H and pad spacing has been changed to 3.65 (center to center) to maintain the same outside pad distance. Since the lens diameter is 1.6 (I didn't see a specified tolerance for that number) I set the hole size to 1.8 Dia. These small changes will increase the drill gap to 0.205mm...
gap.jpg
(violet = Top Terminals, green = Top Comp Outline)
You do not have the required permissions to view the files attached to this post.
Tom

Tomg
Expert
Posts: 1541
Joined: 20 Jun 2015, 14:39

Re: Drill to PAD Clearance

#6 Post by Tomg » 11 Jun 2020, 15:31

If you prefer to keep the 2mm diameter lens opening, the stock pads could be trimmed as shown below to maintain a passable gap size. As seen in the previous example a small amount of terminal-to-pad contact area will be lost, but if you think you would like to try this method I can post a DXF file with instructions that will produce these pad shapes when imported into the Pattern Editor.
2mm.jpg
You do not have the required permissions to view the files attached to this post.
Tom

PaulNewf
Posts: 42
Joined: 20 Jan 2016, 08:33

Re: Drill to PAD Clearance

#7 Post by PaulNewf » 15 Jun 2020, 08:01

Tom,
Both of those look good, I have to ponder the differences.
I will try on my next board order, which is hopefully this month.
Thank you for the detailed drawings, they really clarify the ideas.
Paul

Post Reply