I am user of Orcad PCB editor 16.0. while setting Ref. designator i found its size is too big. I am not able to place near comp. due to high density and the Ref. Des. size is too big. If I make down the size I can fit them in position. I tried to change by selecting all text only and then Setup> Design parameter> Text option. But I am not getting Apply button highlighted. so nothing is changing on the board. Pl s let me know how to change the text size of designator in design.
Set the visibility to show just the text that you want to change the size of, like Ref Des / SilkScreen Top, and the Board Geometry / Outline (to get the board extent) Then, from the menu, Edit>Change, in the Options tab, check the box to the left Text Block, set the required Text Block, with the "default" text block sizes you won't be able to go much lower than Text Block 4 for SilkScreen, drag a box around the items (or the entire board) and right-click>Done (or F6 is the default function key for Done) and the change will be applied. Any items that have the same text block size as the specified "to" size will be logged to the command window.
In reply to oldmouldy:
In reply to Prasanna:
Another way to change text sizes generally is to change the text block settings.
If you want to change textblock 4 to something else everywhere it is used on the board you can use Setup, Design Parameters, Text and click Setup Text Sizes.
You could also just type "define text" at the command prompt or create a shortcut "funckey F7 define text"
In reply to Ejlersen:
In reply to dsfii:
In reply to redwire:
If you are using 16.6 you can also in Placement Edit mode (Setup - Application Modes) hover over the symbol and use right click - Refresh symbol instance.