Altium Layer Configurations

[ondo]

Every time I start a PCB I edit the layer names and pairings to fit my usual "build". I've been looking if there's a way of setting it to the default, at least of changing the default enabled layers and its names, but can't find it anywhere. Any clues??

[T3sl4co1l]

Templates maybe?

I don't know if there are even PCB templates the way there are schematic templates... I mostly copy and paste the same starting file and go from there

Tim

[free_electron]

scripts

Code: [Select]

Private Sub LayerLabeler
    dim TheBoard                                                                ' Storage for the board object
    dim TheLayerstack                                                           ' storage for the layerstack object
    dim TheLayer                                                                ' storage for the layer object
    dim x                                                                       ' integer variable

    set TheBoard = pcbserver.GetCurrentPCBBoard                                 ' Let's grab the board handle of the current PCBDoc
    set TheLayerstack = TheBoard.layerstack_v7   ' layerstack                   ' and snatch the layerstack associated with TheBoard.
    for x = 1 to 32
        set TheLayer = TheLayerstack.layerobject_v7(Ilayer.MechanicalLayer(x))  ' Now let's grab a layer in the stack, pointed to by x

        TheLayer.MechanicalLayerenabled = true                                  ' We'll turn it on
        TheLayer.isdisplayed(TheBoard) = true                                   ' and show it
                                                                                ' The statements below will turn it back off
                                                                                ' if it is not in the 'approved list'. Doing it this way saves lot's
                                                                                ' of keyboard pounding.

        select case x                                                           ' Switch depending on the Mechanical layer number :
            case 1
                 TheLayer.name ="[M01] 3D Part Outline"
            case 2
                 TheLayer.name ="[M02] Board Outline"
            case 3
                 TheLayer.name ="[M03] ConCoat Top"
            case 4
                 TheLayer.name ="[M04] ConCoat Bottom"
            case 5
                 thelayer.name ="[M05] Coverlay Flex Top"
            case 6
                 thelayer.name ="[M05] Coverlay Flex Bottom"
            case 7
                 thelayer.name ="[M07] Stiffner Top"
            case 8
                 thelayer.name ="[M08] Stiffner Bottom"
            case 11
                 TheLayer.name ="[M11] PCB Notes Top"
            case 12
                 TheLayer.name ="[M12] PCB Notes Bottom"
            case 13
                 TheLayer.name ="[M13] Assy Notes Top"
            case 14
                 TheLayer.name ="[M14] Assy Notes Bottom"
            case 15
                 TheLayer.name ="[M15] Courtyard Top"
            case 16
                 TheLayer.name ="[M16] Courtyard Bottom"
            case 17
                 TheLayer.name ="[M17] Titleblock Top"
            case 18
                 TheLayer.name ="[M18] Common Data TOP"
            case 19
                 TheLayer.name ="[M19] Film Markers"
            case 20
                 TheLayer.name ="[M20] Titleblock Bottom"
            case 21
                 TheLayer.name ="[M21] Common Data Bottom"
 end select
next
end sub

you can do the same for the electricals by altering the iterator :

Code: [Select]

 private sub ElectricalStack_LongNames
       dim Theboard
       set theboard = pcbserver.GetCurrentPCBBoard
       dim iter
       set iter= theboard.electricallayeriterator
       dim x
       x = 0
       while iter.next
         x = x + 1
         iter.layerobject.name = "[L"+ right ("00"+cstr(x),2) + "] "+ layer2string(iter.layerobject.layerid)
       wend
    end sub

[JDubU]

Menu item:  DXP >> Preferences

Choose:  System >> New Document Defaults

Select from list on right:  PCB

Click on '...' button that appears on right side of selected line to browse to a default pcb file

[free_electron]

Templates maybe?

I don't know if there are even PCB templates the way there are schematic templates... I mostly copy and paste the same starting file and go from there

Tim

yes there are. they are tied to sheets. the setup is more complicated than schematic though as you deal with top and bottom views.

[ondo]

Menu item:  DXP >> Preferences

Choose:  System >> New Document Defaults

Select from list on right:  PCB

Click on '...' button that appears on right side of selected line to browse to a default pcb file

Thanks! worked like a charm.