Stats

Locked Locked
Replies 4
Subscribers 165
Views 16491
Members are here 0

Drill Chart Rectangle Line Width

Hey all,

Being fairly new to PCB Designer, I'm going to try and be detailed in what I've tried and what has worked for some of my related problems in hopes that it will help others just starting with the tool. I've found other posts give options/answers, but I'm unable to find where these sections/options are since I'm not fluent in PCB Designer yet.

I am using OrCAD PCB Designer v16.2. I have a design that I'm trying to create the artwork for and I am having many 0 line width problems. I solved the text problems by changing the Photo Width field entries to non-zero numbers in Setup-->Design Parameters-->Text Tab-->Setup Text Sizes. I have solved line width problems by making the Class/Subclass active for the line in question and using Edit-->Change, to change the line width and then selecting the particular line to change its properties.

The current problem that I haven't been able to solve is the rectangle around the drill chart. It is a 0 line width. The warning I get in the photoplot.log is "WARNING: rectangle or unfilled shape composed 0 width line found at (3633.0 -1050.0)... ignored!" I created the drill chart using Manufacture-->NC-->Drill Legend and used the default-mil.dlt template. I fixed similar problems in the drill chart with the text and lines using the above steps, but when I try the solution above that I applied to lines to the rectnagle around the drill chart, it doesn't work because it says "Rectangle line width cannot be changed". I tried another poster's suggestion by changing the field "Undefined line width" in the Manufacture-->Artwork window from a 0 to something non-zero, but that didn't seem to help.

Ideally, I'd like to change the template, so I don't have to fix this problem every time in future designs, but temporarily solving it for this design is my main goal right now. Any thoughts? Thanks.

--Mark

steve over 16 years ago

Search for default-cm.dlt (or default-units.dlt) normally under install_dir\share\pcb\text\nclegend. You can custom modify your nc drill table. I don't think you can modify the line width though.
When using an undefined line width (artwork settings) make sure you define a width for each artwork. That might be your issue.
Cancel
Vote Up 0 Vote Down

Cancel
melview1 over 16 years ago

Brilliant!
I didn't know the 'Film Options' field in the Artwork Control Form changed depending on which film was selected. I thought they were just global parameters. That's why when I changed it before, it didn't seem to fix the problem. I changed all of my films to 4 mil undefined line width and I still get the warnings when generating the artwork, however it doesn't ignore the lines anymore, it uses 4 mil width and they show up on the artwork. Thanks Steve.
I had previously found where the default-mil.dlt template that I'm using is, however I'm not sure how to open it to modify it. Any suggestions?

--Mark
Cancel
Vote Up 0 Vote Down

Cancel
steve over 16 years ago

Mark

Use notepad / wordpad.

Steve

Brilliant!

I didn't know the 'Film Options' field in the Artwork Control Form changed depending on which film was selected. I thought they were just global parameters. That's why when I changed it before, it didn't seem to fix the problem. I changed all of my films to 4 mil undefined line width and I still get the warnings when generating the artwork, however it doesn't ignore the lines anymore, it uses 4 mil width and they show up on the artwork. Thanks Steve.

I had previously found where the default-mil.dlt template that I'm using is, however I'm not sure how to open it to modify it. Any suggestions?

--Mark
Cancel
Vote Up 0 Vote Down

Cancel
edhickey over 16 years ago

SPB 16.3 will support user defined line width for the drill legend outline.The following record will be added to the .dlt file
; ?LineWidth
; Width of lines used to draw the legend table in the units as indicated by ?Units.
?LineWidth N
Cancel
Vote Up 0 Vote Down

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.