here is the item from Protels site,  dont bother with the hole detector add
on, it only gives you the co ordinates,  this will find them as errors

12) Item No. 2118 - Last revised 30-Jul-2001
How can I detect overlapping pad and vias on my PCB?

Protel Knowledge Base
Item - 2118
Logged: 7-Jan-2000   Revised:30-Jul-2001
Item categories: PCB Design
Products affected: Protel 99 SE (SP4);
Operating systems affected: Windows 2000;95;98;NT;


Query: How can I detect overlapping pad and vias on my PCB?

Answer: You can set up a Clearance Constraint design rule to detect
overlapping pads and vias.
To do this:

1) Add a new Clearance Constraint design rule in the Design Rules dialog.
2) In the Clearance Rule dialog set the Filter to Object Kind, and enable
the Vias, Thru-hole Pad and Smd Pads check boxes.
3) Repeat this for the second Filter in the lower part of the Clearance Rule
4) Set the Minimum Clearance to 0 mils.
5) Select Any Net in the drop-down list in the bottom-right of the Clearance
Rule dialog. This means the rule will test for pads/vias on the same net, as
well as different nets.

Any pad or via that touches another pad or via will now be flagged as a
design rule violation.

Warning - This specific rule has higher priority over normal clearance rule
for vias/pads and can allow a clearance violation to go unnoticed so it is
advisable to disable this rule before doing a final DRC check for
fabrication. This occurs when the overlapping pads/vias rule has a Minimum
Clearance set to 0 mils and then doing a DRC for say Whole Board rule and
overlapping pads/vias rule will result in a clearance violation that goes
unnoticed for pads and vias only.

Therefore it is recommend that if you intend to use the above described
technique for detecting overlapping pads and vias, disable the specific rule
when performing a general Design Rule Check.

is performed separate to the Whole Board design rules or other rule scope
that does not have an Object Kind type.

Mike Reagan
Frederick MD

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to