ECO Generation Tab
The ECO Generation tab in the Project Options is a great place to keep particular items from being ripped out of the PCB. For example, a schematic has been loaded with some directives and classes, but is not totally complete. Therefore, to work the PCB properly, more information needs to be added, but then the ECO tries to rip that information back out of the PCB. The ECO Generation tab can fix that for you. Customize the list according to your particular project, but very common items to turn off are...
1. Add Rooms
2. Remove Rooms
3. Remove Component Classes
4. Remove Differential Pair
5. Remove Net Classes
Do NOT use the Comparator tab
Everything that can be done in the ECO Generation tab can be done in the Comparator tab, yet it is inferior and potentially dangerous.
First of all, note that in the ECO Generation list above, there are toggles for both Add and Remove. In certain instances, there are even Change options. With Rooms for example, in the Comparator tab, there is only Extra Room Definitions. This disables room changes from both directions with only one option.
Also, when using the ECO Comparator tab, you are disabling only the output to the ECO. In other words, Altium will still see that there are differential pairs in the PCB that do not exist in the schematic, but will simply ignore that. There is also an nice popup that lets you know that there are differences in the design, but it has not made an ECO since the differences have been deliberately turned off. This is not so with the ECO Generation tab. When those items are turned off, they are OFF. There is no check, no warning, no nothing to let the next person working the design know that they may not be getting new information from the schematic to the PCB.
Project Parameters
If you are not currently using project parameters, start using them. They are so tremendously helpful. How many times have you had to change the exact same number in 4-10 different places all over the board for a PN change or a revision change? Project parameters can eliminate that. Under Project Options, the empty Parameters tab is near the end. Simply add parameters by Name and by Value. The Name is how the parameter is called in the design, the Value is what will show. Follow these basic steps to see an example of setting a single PN for both PCB and all schematic sheets in the design.
1. Click Add... and set the Name to PrjPN and the Value to 123-456
a. Note that the extra "Prj" prefix ensures that a System Parameter is not accidentally used. If a System Parameter name is used in the Project Parameters, this will fail.
2. Add a string to the schematic. Instead of typing the text, use the small pulldown of special strings and find the new PrjPN parameter like so...
3. Copy this string to multiple pages and places within the schematic.
4. In the PCB add a string and use the pulldown to find the same parameter.
a. Note that in the PCB the sting will be preceded by a period as opposed to the equals sign that is used in the schematic.
5. Copy this string to multiple places and layers within the PCB.
6. Ensure that Convert Special Strings in on for both the schematic and PCB.
a. The schematic checkbox is global and is under DXP->Preferences->Schematic->Graphical Editing
b. The PCB checkbox is local to the PCBDoc and is under View Configurations (shortcut key "L"), under the View Options Tab.
7. At this point, 123-456 should show in all locations. Change the parameter value once in the Project Options and the new value will be reflected in all locations.
a. Altium may need a refresh to display the new numbers. Simply hit the End key on the keyboard to force a refresh.
So the best part about keeping a master PrjPCB file is that it is possible to copy/paste all the commonly used Project Parameters into a new PrjPCB file!
No comments:
Post a Comment