| T O P I C R E V I E W |
| CPS |
Posted - 18 Aug 2009 : 13:44:57
I have a number of single side (no-hole) pads that are sprung pin test points / microcontroller programming points. Therefore during gerber output I want the solder resist to be generated as normal, but the solder paste mask to ignore these pads - so no paste is put on them during manufacture.
How do I set this at design time, rather than post-editing the gerber which is a pain!
|
| 4 L A T E S T R E P L I E S (Newest First) |
| CPS |
Posted - 19 Aug 2009 : 16:03:02
Thanks, all is clear now. I was trying to work out how to alter the way the 'automatic' resist was generated, but now see that if you generate your own layer you can do whatever you want to it!
|
| Iain Wilkie |
Posted - 18 Aug 2009 : 16:23:53
Simply create extra layers for paste and resist in the layer types and then follow Davids instructions....
Type in "layer types" in the help file for info.
I use this all the time to make alterations to resist and paste masks for edge connectores etc etc..
Iain |
| CPS |
Posted - 18 Aug 2009 : 14:48:54
But I don't normally have a solder resist /paste layer, as the gerber is just generated automatically from the top copper layer. |
| DavidM |
Posted - 18 Aug 2009 : 14:14:53
If you find the pad style that these pads use (in the Design Technology dialog), select the style then click 'Add Exception'. On the padstyle exception dialog, set the layer to your top paste layer, and the width to zero.
This 'hard-wired' size will then be used in preference to the normal method of undersizing all the pads, and hence suppress those pads from the plot completely.
You can use the same technique if you want to apply a specific paste size to a padstyle, for example if the standard undersize would make a particular padstyle too small on the paste plot you can add an exception to make them a little bigger.
|
