Add hole to library in cadstar

Hi,

do you know how to add a hole to the library in cadstar?

-i go FILE -> NEW SCHEMATIC SYMBOL -> DEFAULTS,

-then i've no idea what to do .

nothing like this is explained in the user manual.

Draw your symbol and add it to your schematic library. Then make your PCB footprint and add that to the component library. Your PCB footprint can be a zero sized pad (I think CADStar allows that) with a drilled hole and probably some silkscreen and assembly layers.

Using Library Manager, open the library where you want the part to reside, Mechanical maybe? Add a new row at the bottom and add a Part Name (also copy this part name into the Definition column). Right click on this row and select Edit Part Definition, under the component and Symbol tabs add your newly created schematic symbol and footprint.

There is assignment table in Cadstar where you can add hole.

As Rob says, add this as a part.

Create a part, perhaps called "Mounting hole 3.5mm" so that you can create other sizes similar.

Use a symbol like a circle or even a screw etc.
Create a component that has a drill the size you want.

For mounting holes with plating through and pad land for screw head contact, make it with the pad the size of the screw head (or larger), drill hole slightly larger than the screw thread and plated through.

For non plated through holes with no lands, make the drill size what you want and the pad size slightly less than the drill size.
This way you still see the hole there and the pad will be drilled away.
(Or you can make it zero sized and use the "show drill holes" option).

You may also like to add a "no routes, no vias" area on top/bottom layers so that mounting standoffs & screws do not damage/contact them.

Also add a reassignment of zero size on both your paste layers so that they do not appear on your paste screen.

Do not bother with reassignments for solder resist layers - provide them 1:1.

Create a series of parts to provide different sized holes (or create 1 part and use alternative components for different sized holes).

Then you can add the part to your schematics, perhaps on a spare sheet I.E. "PCB only stuff" so you do not print them out on a schematic.

That way when you do an ECO, they will not get removed because you have forgotten to use the old way of adding a component ignore file.

To recap:
Create a part with both symbol and component.
add to schematics to allow a better ECO etc.