Stats

  • Locked Locked
  • Replies 4
  • Subscribers 165
  • Views 13349
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

My artwork didnt work as intended....any advice?

hohk

Hi,

 

1. I created a PCB layout with only traces on the top and bottom layer connected to a padstack (modified to be a through hole).  

2. Manufacture> Artwork > Create Artwork (i choose gerber Rs274X, checked bottom and top films). In the end i had a TOP.art and BOTTOM.art.  The photoplot.log shows DRC errors but i ignore it since i only want to test outputing gerber files.

 3. When i import>artwork> TOP.art and choose Class = Etch and Subclass = Top, i get the top trace and the pad (green color). BUT, when import BOTTOM.art, and choose Class = Etch and Subclass = Bottom, i still get the top layer trace and pad only but in a different color (yellow).

 

So,  why cant i get the bottom trece and pads only when i impport the BOTTOm.art? Is my concept wrong?

 Thanks. Attached is my sample board file. Its just a test since i am new to PCB Editor. Hope some one can give some advce.

 

 

wa.zip
  • oldmouldy

    If you open up the Films in Manufacture>Artwork, Film Control tab, you will see that both the TOP and BOTTOM use the TOP subclasses for VIA CLASS, PIN and ETCH, hence you get the data for the TOP output to both films. You need to add the classes for subclass BOTTOM and then remove the classes for subclass TOP from the BOTTOM film.

  • redwire

    As a double-check, here is your board modified with the correct artwork subclasses.

    wa2.zip
  • hohk

     

    Thanks for the advice and pointing out my mistake.

    Another question(s).

    1. If my board has lots and lots of non plated through holes of many different sizes, i have to create padstacks with pads smaller than the drill holes right? Is there a way to position them accurately by typing in coordinates (i have enginerring drawings) rather than using closely spaced grids?

     2.  If one of the through holes have large diameter (15mm), the PCB house said they have to route out the hole, does this mean that they will use a smaller drill bit and just cut along the circumference of the hole to create the hole?

     

    Thanks.

  • steve

    1. You have a couple of options. First is to place using the command line (Edit - Move) select your hole the at the command line type the specific co-ordinate i.e x 1256 1345. You can also use the RMB and snap to a specific point (circle, intersection etc). Or you can move a pad by a specific amount using ix or iy (incremental mode). Ensure your origin is set to a known point.

    2. You can either just add a diameter or raidal dimension to the inner circle and show this on a fabrication drawing or create a nonplated hole that diameter (and leave it up to the fabricator as to how he creates the hole). There is also a NC - Route option that will create a set of routing co-oridnates that the fabricator can use. But to answer your question - Yes that is normally how they route out items.  

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.