Altium new pcb wizard removed?

[AlfBaz]

PCB creation wizard was excellent when you just wanted a simple board but I cant find it anywhere on any version since 17

It use to reside in the files panel before but that seems to be gone also.

Have they really removed it and if so why?

[AlfBaz]

bump

[Gibson486]

I did not know that even existed. What did it do?

[AlfBaz]

I use it for simple stuff, it's quick and simple, cobbling together rudimentary design rules based on entries into it. It's been around since at least 99SE
Here's a link to it on V15.1. The last versions that I could find it in were 17.x
https://www.altium.com/documentation/15.1/display/ADES/PCBMaker_Dlg-Form_BoardWizard((Altium+Designer+New+Board+Wizard))_AD
 

[grosfaignan]

is there any other way to set up PCXB properties as th pcb board wizard do ?

[AlfBaz]

What version are you using? Im guessing it's 18 or higher

[grosfaignan]

18 yes

[AlfBaz]

Sorry for the late reply, had to attend to a few things

What the PCB wizard did was ask some basic questions and from the answers, derive some of the rudimentary design rules and of course create a basic board outline.

So here’s a basic outline of how to do this manually
Add New to Project -> PCB
This creates a PCB doc with a double sided pcb 6000 x 4000 mils with the bottom left corner at 1000, 1000 x/y coordinates from the origin.

Most of what you need to know about redefining the board shape can be found here
https://www.altium.com/documentation/18.0/display/ADES/((Defining+the+Board+Shape))_AD

For a simple rectangular board, I’ll place a horizontal line on mech layer 1, double click it and change its start x,y co-ords to something even like 100,100. This makes it easy to see the length of line by subtracting 100 from the end x value. From there it’s just a matter of adding the rest of the lines to suit.

Note that the bottom left corner of the board is not at the 0,0 origin. Personally I do this so I have room at the bottom and to the left of the board as you cannot draw or place anything in the negative regions

With the board now created you need to set up the layer stack. Design->Layer Stack Manager. Here you set the number of layers. If you need an accurate stack up, refer to your PCB manufacturer for their default stack up and reproduce it here.
There are presets in here but anything greater than 2 layers uses planes. You can change those to signal layers if you want.

You then need to change the design rules. Design->Rules.
Basic rules set by the wizard were routing widths and via sizes
Go in and adjust those to your required min max and preferred values.

I’d suggest you get acquainted with the rest of the design rules as they’re very handy for picking up errors
You can choose which rules are done live (online) by selecting Tools->Design rule check...
Under the rules to check folder you can click on each category and select online or batch with the latter showing up only after running a design rule check by pressing the button in the lower left corner of its dialog box

If there’s anything else you want clarified feel free to ask