I've opened up an existing brd file that I generated using OrCAD PCB Designer Professional v16.5. It appears that all of my parameters remained intact, however, the colors, transparency and brightness of the individual elements look different. Most of the differences aren't bad, they're just different.
The only problem I'm experiencing with this new color scheme is that my silk screen elements are almost completely invisible. You can't really see them unless you place your cursor over the silk screen element that you would like to see. I've even set the color of all of my silk screen elements to bright white in the Color192 screen and toyed with the transparency and shadow settings. The only way I can see the silk screen items is to supress all of the other elements and just enable the silk screen stuff. Even then, the color of the silk screen stuff is very muted and not very bright at all.
Has anyone else seen this or have an idea how to make the silk screen more visible or brighter?
Do you have the photoplot width set to something other then zero for the text size you are using?
Obvious questions.......... You have the silk layer for the ref des turned on and the color set to white or some other std color?
I have a board here that I started in 16.5 and finished in 16.6 and there were no issues with the silk viewing
In reply to TH Designs:
The photoplot width for all of the silk elements are at least 0.25mm wide, most items are wider. When I roll my cursor over the silk screen items, they become visible. If I turn off all other layers and leave the silk screen on, I can see it, but it's very dull. It's weird. I've never had this problem before, and this wasn't a problem last week when I completed the board using v16.5. I'm sure it has to be something really simple, but I haven't stumbled across the solution just yet.
In reply to David Yackman:
It's called Shadow Mode, Display - Color Visibility - Display folder, is shadow mode on ? If so turn it off. This is used during highlight of nets, shadow mode turns everything grey (or dimmed) apart from the highlighted net. There's an icon next to the color visibility one which you may have selected.
In reply to steve:
What is shadow mode used for, or how would I use it to enhance my design experience?
It's as I said before used to dim the rest of the board whilst looking at a highlighted net. It works quite well with cross probe. You can adjust the level of dim / brightness including dim the active layer from color visibility - display folder.
Yeah, shadow mode isn't it. I can turn off shadow mode and everything is pretty bright, with the exception of the silk screen items. I can turn shadow mode on and vary the brightness and transparency of items, but the silk screen items remain unaffected. The only way I can see any of the silk screen is to roll my mouse over the item, then it becomes highlighted and visible. But, just as soon as I move the mouse away from the item, it disappears. I can turn off internal layers of the board which contain copper planes and then I can just faintly make out the silk screen items, but still, it is very dim and weak, even though the silk screen stuff is set to white, which should be highly visible. All of the net names and via names are in white (which is kind of a cool feature in 16.6) and it's very visible, so I'm having trouble understanding why my silk screen stuff isn't. Like I said, when I designed this board using v16.5, this wasn't an issue.
I guess I'll send EMA-EDA an email and see why this is happening. If I get a solution from them, I'll post it here. Thanks guys.
steveTomIt's as I said before used to dim the rest of the board whilst looking at a highlighted net. It works quite well with cross probe. You can adjust the level of dim / brightness including dim the active layer from color visibility - display folder.
I'll have to give it a whirl.
Sort of like the "h" (highlight) and "." (high contrast) keyboard shortcuts in the pre 16.3 versions.
David Yackman I guess I'll send EMA-EDA an email and see why this is happening. If I get a solution from them, I'll post it here. Thanks guys.
Just a thought - are you on the latest 16.6 hotfix ??
Good point. I had some weird things going on until I updated.
Just an update - I've designed three additional boards since I've reported this issue. I haven't had the silk screen problem since. All the new stuff I did looks just fine. I guess something is wrong with the *.brd file on the board I designed in 16.5.
Maybe something in the database was set to make it think a partition was exported but in reality it was not exported. You could try changing the environmental variable DISPLAY_READONLY_INTENSITY to 100 and see if the silkscreen items are displayed like normal. (Setup > User Preferences under the Display Category / Visual folder.)
Of course it is a long shot that this is the case but I had to bring it up.
Hope this helps,Mike Catrambone
In reply to RaylonS:
When using PCB Team Design (Design Partition) that is how it works, features are deemed separately and will still be deemed when the Global and Shape transparency is set to 100% in the Color Dialog form.
Using PCB Team Design, you have the ability to export a partition of just the Silkscreen layers which means that the SILKSCREEN_TOP & SILKSCREEN_BOTTOM subclasses under PACKAGE GEOMETRY, BOARD GEOMETRY and REFDES will be deemed differently in the master design giving you a visual representation of what has been exported and if you attempt to move these deemed elements you will not be able to because they will be owned by the exported partition until the updated are imported back to the master design.
Not sure if the original user that posted the question ever figured out what was going on, there may of been a database issue causing certain elements to be deemed differently than others. I believe he was sending a request to support to see what is going on.