Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
The reply is rather complicated, depending on lots of other factors and how you are designing your board.
However the basis is that you would use a coper pour template after the board has been routed to then allow you to pour a full copper layer onto an electrical layer to use as a gnd plane.
Or when setting up your board to define areas that make up a split plane, perhaps with lots of different voltages on so that in the routers you can select them and pour copper.
Or on routing layers, for after you have routed to add additional copper areas.
You do NOT use Maximise copper.
That is a feature that was available in the DOS version and IMO should no longer be in CADSTAR however some older users are likely to be unhappy with it's removal. Pouring with templates is far superior.
(You are welcome to try it, laugh at the results and then undo it all.)
IMO you need to scour the help files when doing this to fully understand what is happening.
Copper for any copper shape that is unlikely to change..
Template for any copper area connected to pins, carrying current or voltage.When routing a board have any power plane layers as actual poer plane lane during routing, this is changed in the layer stack editor. Then when routing complete turn back to electrical layer and copper pour.
1) Yes turn off "auto pour" as this will repour the entire template after every route. In fact when you start routing a board it will flood fill the entire board after one route.
But do this in the routing configuration (CTRL+T) to turn the function off rather than deselect it in the template. That way when you come to do minor mods at the end you can use auto repour.
Like all the other tools, it has it's time and place to be used and at the start of a layout is not where this one should be used.
2) Set a slither width, this MUST be greater than the outline width.
I.E. your outline width is 10th so make the slither width 10.1th
The reason for this is that when transferring back to CADSTAR an illegal shape can have been created in PREditor (one that includes shapes less than the outline width). Consider the pen width of a pen plotter (which the settings are still based on) and copper cannot be drawn any thinner than the pen (outline) width.
Yes copper pour will adhere to your DRC rules, the settings are for above those rules.
I.E. if your DRC is set for coper to pad at 0.008" and you set the clearance to be 0.005" then it will be poured to within 0.008" of the pad (following the DRC).
Use additional isolation to increase the clearance between the copper and routes/pads that are not connected to the net that the copper uses. Often a user will use the same spacing so zero is put in this setting.