Stats

State Not Answered
Replies 9
Subscribers 161
Views 8712
Members are here 0

unexpected DRCs after changing mechanical pads of USB-C connector

I am refering to the USB-C connector JAE DX07S016JA1. It's symbol contains a non-plated hole and slot. presumably for improving mechanical ruggedness.

The symbol is drawn with imperial units, but our pcb manufacturer uses metric drills, which are avaiable in 50µm steps of diameter.

So I made a backup copy of the symbol (the .dra-file) from within the file-explorer. Then I opened it, identified the pad-files of the hole and the slot. I opened both pad-files, adjusted and changed them to metric units and saved them with a different name, refering to the metric units.

In the symbol, I replaced the hole and slot (pins) with the newly created pads and saved the .dra-file with the same name as before.

In the layout I chose "Placement edit" as application mode, selected the USB-C connector's symbol and in the context menu chose "Quick utilities" / "Refresh symbol".
But now a lot of new DRC errors emerged, even several Pad Soldermask to Pad Soldermask Spacing errors between pads that I did not even touch!

I tried to find out about possible reasons for new DRC errors in the documentation "Help" / "Documentation" burger menu "Allegro PCB Editor" / "Allegro User Guide" / "Creating Design Rules", but did not suceed.

Can you guide me into the right direction?

0 steve over 2 years ago in reply to Manfred1

You have to have a valid maintenance contract to get the latest release. Can you maybe post the filename.dra footprint here so it can be reviewed to see if there are any issues with it?
Cancel
Vote Up 0 Vote Down

Sign in to reply

Verify Answer

Cancel
0 Manfred1 over 2 years ago in reply to steve

I would be happy to upload the file, but it doesn't work. Files ending in .dra are not accepted. Files ending in .png seem to work, but in reality do not.
Cancel
Vote Up 0 Vote Down

Sign in to reply

Verify Answer

Cancel
0 Manfred1 over 2 years ago in reply to steve

con_usbc24_dx07s016ja1_s_r_t.txt

I changed the ending from dra to txt to be able to upload the file. The file content remained unchanged. Please reverse file ending from txt back to dra before trying it out.

Kind regards

Manfred
Cancel
Vote Up 0 Vote Down

Sign in to reply

Verify Answer

Cancel
0 steve over 2 years ago in reply to Manfred1

I've placed the connector into a board file and I see a couple of errors related to the Mechanical Drill Hole to Pin Spacing which you probably can't do anything about if you have followed the manufacturers guidelines so I added a property to the symbol (open the filename.dra then Edit - Properties, In the Find Pane. change the Find by name dropdown to drawing and add NODRC_SYM_SAME_PIN, Apply and OK). Save the footprint and refresh this in the board file and I no longer see those DRC's. In regard to the soldermask errors I'm not seeing any so check the values you have set in either Constraint Manager - Manufacturing - DFF - Mask or Annular Ring or under Setup - Constraints - Modes - Design - Soldermask and see if that helps.
Cancel
Vote Up 0 Vote Down

Sign in to reply

Verify Answer

Cancel

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.