Suggested schematic check DRC settings for Tools>Verify in DxDesigner

Question

I am using DxDesigner for the first time (9.2). When running a Design Rules Check (DRC) there are many rules that can be applied. Many of them make sense to check, e.g. "Property name exceeds maximum length". Others are giving me trouble, e.g. Un-driven Net is an error if I enable it when a net is driven by a transformer with pin type analog. Which ones do you use? Disable? Check, but often ignore the notes or warnings?

Updated 11/23/2010: Under Connectivity here are some I had questions on.

drc-101 Output and bidirectional pins connected together
drc-102 Output and tristate pins connected together
drc-103 Un-loaded net
drc-105 Un-driven Net
drc-106 Multiple Output Drivers
drc-116 Output directly connected to Power or Ground

Note that I am not doing circuit simulation.

Answer 1

I can answer for Altium, and maybe you can translate to DxDesigner.

I pay heavy attention to the group of rules labeled "Electrical": clearance, short-circuit, un-routed net, and un-connected pin. I also pay attention to minimum trace width, minimum annular ring, minimum hole size, silkscreen over component pads, minimum soldermask sliver, and net antennae.

I totally ignore everything in the groups "Testpoint," "SMT," "High Speed," "Placement," and "Signal Integrity." I bet I'll need to worry about those eventually, but they haven't hurt me yet (so far as I am aware).

Answer 2

un driven nets, net mismatch, no output, two inputs and so on are DRC errors from the schematic checks. They can be useful and bring your awarness to certain areas.

Trying to fix each one individually can take some effort, but you are on the right track in identifying the issue.

In my 10 years of various cad packages (mentor, altium, cadence/orcad) I have never used the full schematic DRC. Either I down grade those errors to warnings, or ignore them, depending on the job (for example aviation you cannot ignore them!)

The most useful schematic DRC's are net name checks (review this often V5+ is not V5 and so on even if you intended it to be so), unconnected nets (force you to place a no connect object), and nets with only one connection. Reviewing these three I have found to be most useful, as many projects I have been caught out on subtle typos on net names not being connected, are parts that look schematically connected but are not (Altium I am looking at you).

So do review the net name summary from the checker and ensure all is well, and check for unconnected nets! Not sure how DxDesigner handles netnames, but I have been burnt with Orcad in the past, so always stick to short net names with no spaces or punctuation.

Answer 3

Here's my working list.

Migration are all on:

drc-001 Property can't be mapped to Common Properties   ^(~?[a-zA-Z_0-9+-@.# ]+)$   Error
drc-002 Invalid net name format ^(~?[a-zA-Z_0-9+-.]+)$  Error
drc-003 Invalid property value format       Error
drc-004 Invalid symbol name format  ^(~?[a-zA-Z_0-9+-]+)$   Error
drc-005 Property name exceeds maximum length    40  Error
drc-006 Property value exceeds maximum length   80  Error
drc-007 Net name exceeds maximum length 120 Error
drc-008 Symbol name exceeds maximum length  120 Error

Electrical doesn't check voltage and power

drc-201 Open collector pin not pulled up        Error
drc-202 Open emitter pin not pulled down        Error
drc-206 Tristate buffer not pulled up or down       Error

Integrity

drc-401 Missing symbol property                         Error
drc-402 Missing symbol pin property            Error

(change the Properties to the column you are using, e.g. ITEM. If it is multiple words, put double quotes around it). Since I'm not using Links these may not be useful

drc-820 Isolated link       Error
drc-821 Un-named link       Error
drc-822 Multiple destinations       Note
drc-823 Link and net naming consistency     Warning