Altium Layer Configurations - Page 1
Forum section: electronics / general

author: ondo
author_rank: Contributor
timestamp: November 25, 2014, 10:48:58 am
content: 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??

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 25, 2014, 04:11:28 pm
content: 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 thereTim

author: free_electron
author_rank: Super Contributor
timestamp: November 25, 2014, 04:24:57 pm
content: scriptsCode:Private Sub LayerLabelerdim TheBoard ' Storage for the board objectdim TheLayerstack ' storage for the layerstack objectdim TheLayer ' storage for the layer objectdim x ' integer variableset TheBoard = pcbserver.GetCurrentPCBBoard ' Let's grab the board handle of the current PCBDocset TheLayerstack = TheBoard.layerstack_v7 ' layerstack ' and snatch the layerstack associated with TheBoard.for x = 1 to 32set TheLayer = TheLayerstack.layerobject_v7(Ilayer.MechanicalLayer(x)) ' Now let's grab a layer in the stack, pointed to by xTheLayer.MechanicalLayerenabled = true ' We'll turn it onTheLayer.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 1TheLayer.name =" 3D Part Outline"case 2TheLayer.name =" Board Outline"case 3TheLayer.name =" ConCoat Top"case 4TheLayer.name =" ConCoat Bottom"case 5thelayer.name =" Coverlay Flex Top"case 6thelayer.name =" Coverlay Flex Bottom"case 7thelayer.name =" Stiffner Top"case 8thelayer.name =" Stiffner Bottom"case 11TheLayer.name =" PCB Notes Top"case 12TheLayer.name =" PCB Notes Bottom"case 13TheLayer.name =" Assy Notes Top"case 14TheLayer.name =" Assy Notes Bottom"case 15TheLayer.name =" Courtyard Top"case 16TheLayer.name =" Courtyard Bottom"case 17TheLayer.name =" Titleblock Top"case 18TheLayer.name =" Common Data TOP"case 19TheLayer.name =" Film Markers"case 20TheLayer.name =" Titleblock Bottom"case 21TheLayer.name =" Common Data Bottom"end selectnextend subyou can do the same for the electricals by altering the iterator :Code:private sub ElectricalStack_LongNamesdim Theboardset theboard = pcbserver.GetCurrentPCBBoarddim iterset iter= theboard.electricallayeriteratordim xx = 0while iter.nextx = x + 1iter.layerobject.name = "[L"+ right ("00"+cstr(x),2) + "] "+ layer2string(iter.layerobject.layerid)wendend sub

author: JDubU
author_rank: Frequent Contributor
timestamp: November 25, 2014, 04:26:27 pm
content: Menu item: DXP >> PreferencesChoose: System >> New Document DefaultsSelect from list on right: PCBClick on '...' button that appears on right side of selected line to browse to a default pcb file

author: free_electron
author_rank: Super Contributor
timestamp: November 25, 2014, 04:38:58 pm
content: Quote from: T3sl4co1l on November 25, 2014, 04:11:28 pmyes there are. they are tied to sheets. the setup is more complicated than schematic though as you deal with top and bottom views.

author: ondo
author_rank: Contributor
timestamp: November 26, 2014, 08:25:52 am
content: Quote from: JDubU on November 25, 2014, 04:26:27 pmThanks! worked like a charm.