Update: This tutorial is valid for the DesignSpark PCB version only - there is a built in support of slotted holes for the DS PCB Pro version, see below following replies to this tutorial.
Unfortunately there is still now no official support for slotted holes - just some workarounds after more than 4 years ??
I know this instructional written before
but I think you can do the job much easier.
I hope it is helpful for some customers.
Here we have a modern RCA connector with slotted holes. First create a part with the symbols outlines and oval pads with enough size to enable functional annular (min. 8 mil on each size, the more the better). Write the dimension of the slotted hole in the documentation layer and it's shape, makes it easier to repeat this in the board (and not to forget).
In the board draw a border outline with Add Border Rectangle and make the left and right side to an arc 180°. Change the width in the properties to the minimum milling tool width of your manufacturer, can be 10-20 mil in my experience, and adjust the size of the board outline to fit in the dimensions of the documentation layer, if necessary change grid step size. Otherwise the resulting hole will be too big.
Change the properties of the board outlines to plated. This is important for the manufacturer to platen even the slotted holes.
Set the spacing rules for board to 0 for all items. This is important to get the pads connected later. It is sufficient to just set the spacing to less than the annular region but a few mil spacing is not very helpful so set all to 0.
Now when you like in the example have a copper area filled with GND, the GND pin is connected while the other pin is connected to a different net - this is what you want.
Now the very easy part comes - you don't have to output a different layer - all data is put in the appropriate drill files when you just select in "settings" of Output Manufacturer Plots in the drill file to give plated and unplated board files:
That's it. No layer type needed, no special layer, no manual work to give to your manufacturer (separate file). To avoid DRC check problems you should disable following errors:
You only have to be aware, that you have enough space in your project to all board line objects (manuallly) and if you have unplated drill holes the poured copper area may touch these holes. This can be avoided to use round pads for the same job with pad size and hole size to the desired size (gives a warn dialog you can omit) to keep the distance to any additional mounting holes. See the white line showing the pad as replacement for the unplated drill hole (green line).
I hope this guide helps. And I hope the development team would extend the pad design dialog with different size of oval pad and size parameters for oval drill (which is then a mill instead of a drill). Could be more easy !
Please sign in to leave a comment.