| Author |
 Topic  |
|
|
holdstoc
United Kingdom
2 Posts |
 Posted - 19 Dec 2013 : 17:19:42
|
In the component library I've made a custom SMD pad in the approved way (odd-shaped copper area linked to a smaller SMD pad), and as Easy-PC won't generate solder resist and paste areas from this copper area I've added these manually. However, when the footprint is used on a PCB the solder paste section for the custom pad isn't there. The solder resist area ports across from library to PCB OK, and the solder paste areas from normal SMD pads are all present and correct, it's just that anything I add manually to the footprint solder paste layer disappears once it gets to the PCB stage.
I'm pretty sure I've got everything set up OK (layers and layer types are all defined), but this one's got me stumped. I have a workaround, which is to add the paste area at the PCB stage, but this is a pain as it's independent of the footprint. I don't think it's a corrupted design file or one-off quirk as this is the second Easy-PC design I've had this trouble with.
Any help gratefully received. I have my hand poised within slapping distance of my forehead, just in case I've done something stupid here. |
|
|
edrees
United Kingdom
779 Posts |
Posted - 19 Dec 2013 : 17:26:39
|
Hi,
EPC will generate solder paste and solder resist automatically during your Gerber plotting stage.
For complex pcbs you can add these layers (and see them on your design) in the Design Tech files. If added in this manner you can edit these layers and make further "exceptions" during the plotting phase. Little bit tricky to begin with, -but very powerful when fully understood. |
 |
|
|
nigle
United Kingdom
45 Posts |
Posted - 19 Dec 2013 : 17:28:07
|
| Does the layer name match EXACTLY between the part definition and the one in the PCB? There could be a typo, such as a double space, in one of them which will cause EasyPC to ignore the layer when loading the part. |
|
|
|
holdstoc
United Kingdom
2 Posts |
Posted - 20 Dec 2013 : 10:13:40
|
Thank-you nigle. I thought I checked the layer/type names, but I went back and double-checked: I had Layer Types named "Solder Paste" and "Paste Mask". Giving these the same name cured the issue <slap to forehead>. I do note that the expansion rules on paste and resist layers only seem to apply to proper pads, so any shapes created only on the paste or resist layers need to be manually adjusted accordingly. That's another reason to set the paste and resist layers to the same size as the copper pads, and let the PCB manufacturer sort out the expansions.
I may suggest to the boss that an Easy-PC style sheet be created, as currently new designs can use library parts created by different engineers over the years, and the layer names are inconsistent. With standard pads that doesn't seem to matter so we've mostly been getting away with it.
Thank-you too edrees, I didn't know about the exception capabilities in the plotting, that sounds very handy so I'll be sure to learn all about that. It's always nice to know about options. |
|
|
| |
Topic |
|
|
|
Custom SMD pads: paste layer disappears.