Drill hole count mismatch in drill chart and Gerber output

Status
Not open for further replies.
R

rsashwinkumar

Member level 4
Joined
Jun 25, 2011
Messages
70
Helped
11
Reputation
22
Reaction score
11
Trophy points
1,288
Visit site
Activity points
1,825
Hi all,

I am using Orcad Layout Plus for my PCB layout. In the drill chart of the layout, the number of 10mil drill holes it shows is higher than the number of holes it shows in Auto->Create Reports-> Drills.
The PCB manufacturer also had reported the same problem saying the number of 10mil drill holes found in the Gerber is lesser than the number shown in Drill chart.

I have been trying to debug this issue but have not found what the problem is.

Has anyone faced the same problem, or someone knows the reason for this? Or can someone help me on how to start to debug this issue?

Thanks in advance!
 

It might have something to do with plated vs. non-plated through holes. I've run into this problem in PADS, where it lets you shoot yourself in the foot by defaulting to not put non-plated holes in the drill file.
 
Thanks for your reply!
The 10mil holes I have are all plated holes. None of them is non-plated. What else can cause this issue?

Is it possible to get info about the holes shown in drill-chart? I was thinking if the location of holes in drill chart can be obtained, I can compare with the hole location obtained from Auto->Create Reports and identify the holes with this discrepancy. Any idea if that is possible?
 

@Mattylad : I tried to place two holes on top of each other, but still it counted as two separate holes both in drill chart and in drill report. So I am not sure if that could be the problem.
 

Can you make a drill drawing, showing a marker where the hole is and then visually count them up and compare them to your design.

BTW is the drill chart automatic or just manually added text?
 
I tried to place two holes on top of each other, but still it counted as two separate holes both in drill chart and in drill report. So I am not sure if that could be the problem.
Click to expand...
But the doubled drill hole is usually deleted during NC file generation. So this could well explain the count mismatch. There could be also misplaced drills outside the board area.

Usually, if you have any doubts about the gerber and NC data, you'll check it visually in a gerber tool. If the design isn't too huge, you would see missing drills. Ultimately, advanced gerber tools have various check features to detect vias with missing drills or even verify the gerber data against a PCB netlist.
 
The drill chart is automatically generated in ORCAD. It gets updated whenever a new via is added or deleted.

@FvM : Then I should probably check the vias individually and see if I have placed two vias at the same place by mistake.
 

Newer software caters for this with on the fly reconnect. Orcad layout is old and was ditched by Cadence in 2008, the newer Orcad PCB Editor (cut down Allegro) is better and more up to date.
 
Hi,

Thanks for your replies. I finally deleted all the vias, and placed them manually and got it working. But still trying to look into the old file if I had placed any vias on top of each other.
 

Orcad layout allowed this to happen, the excellon file should be correct (I have never known one not to be)...In my world the best way to avoid this is don't put a drill table up, tell the manufacturer to use the excellon files.....
As for drill drawings...they use to be done so the manufacturer could digitise them and create an NC drill file (on some twee little tapes), nowadays who is going to use them except for the simplest of boards! with IPC-D-356 nets to check against or even better ODB++ they are totally redundant, try using a drill drawing for a HDI board with 6 layer pairs and a few thousand vias....to much redundant information.
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…