| Author |
 Topic  |
|
|
PaulR
United Kingdom
9 Posts |
 Posted - 10 Jan 2014 : 07:34:13
|
Hi, not really a new issue - Iain Wilkie has already raised this (see except below).
DRC checking for component - component spacing is not sufficiently intelligent and has been an irritation for year. Because components come in all sorts of body shapes and sizes it's too much to expect an automatic check to work well in many circumstances. I support Iain's request for the ability to create specific outlines. Might we need the ability to have different outlines on <top> and <bottom>? e.g. for a potentiometer whose shaft goes through the PCB, so it has its body on one side and the shaft/nut on the other.
Iain's request:
2. The DRC for proximity really needs some work. I find I'm not really using it anymore due to the number of false positives. How about having an optional extra layer in PCB footprints which defines the physical footprint of the component for DRC / proximity checking purposes? This would probably be required to be some sort of closed shape. The DRC needs to be able to check proximity between polygons.
3. AFAIK ODB++ does not automatically generate solder mask / resist, the options to do this automatically as in the gerber generator would be great.
4. Optional layers for solder paste / solder resist in pcb footprints, but while somehow still maintaining the excellent way of automatically generating this output (should the layers not be defined).
So to summarise for 2,3&4 in the PCB footprint creation there would be three extra checkboxes:-
- explicit physical outline shape for DRC purposes
- explicit solder resist
- explicit solder mask
PaulR
|
|
|
DavidM
United Kingdom
458 Posts |
Posted - 10 Jan 2014 : 08:50:41
|
There is already a method of doing this in the application that I believe should cater for what you need.
In a PCB symbol you can create a new layer type (or alter an existing one if appropriate) and enable its "Placement Shapes" property. Then create a top and bottom layer that use that layer type, perhaps "Top Body" and "Bottom Body". Now add the required shapes on those two layers to represent the physical elements of the component body on each side. So you could have a large circle on the top side for the 'can' of the potentiometer, and a smaller one on the bottom side for the shaft.
Now in your PCB design you will need to make sure you have the same layer type and layers as in your symbol, so that those shapes have somewhere to live. You can either do this by editing your technology file used to create new PCB designs, or by directly editing in the Design Technology dialog for an existing PCB.
Having done that, when you add (or update) the component that uses that potentiometer symbol, it should bring across its placement shapes. Now when you run DRC, it should recognise those shapes as being your definition of the component body on each side of the board, rather than use any 'default' method such as the silkscreen outline or bounding box.
In theory there is no limit to the complexity of how you construct your placement shapes in the symbol. You can have circles, rectangles, polygons, you can have multiple shapes, and even shapes with cutouts.
I hope this covers what you need for your checking purposes.
David. |
 |
|
| |
Topic |
|
|
|
Explicit component outline for DRC purposes