Minimum annular ring Altium desing rule?
Kamil , 04-09-2024, 06:43 AM
Hi! Have you created the rule for vias or pads where there are different annular value for top/bottom layer and inner layers? I cannot figure it out..... 😦 For example i have values for outter layers 8 mils and inner layers 5 mils, i'd like to have minimum annular ring rule for those, layer depended, values...
QDrives , 04-10-2024, 07:13 PM
Outer layers bigger than inner layer? Usually it is the other way round.You create a rule with a custom query and use OnOutside and/or OnInside and set the corresponding value.This requires 2 rules - one special and one standard.
Kamil , 04-10-2024, 10:20 PM
Yes, outter layer has bigger minimal annular ring because of large drill value... Thank you, I will try it soon. And is there rule to set minimal annular ring depending on layer copper height defined in stackup? For example, manufacturer has 5 mils for 35um but 8 for 70um... Can't now remember exact values but I think I am not wrong.
Kamil , 04-10-2024, 10:25 PM
Note that objects placed on the Multi-Layer layer will not be returned by the OnOutside query keyword. Pad and Via are on multilayer, so... It doesn't work. I remember now I tried that. Look: https://www.altium.com/documentation/altium-designer/layer-checks-pcb-layout-query-functions#onoutside
Kamil , 04-10-2024, 10:27 PM
I will try: ExistsOnLayer('Top Layer') Or ExistsOnLayer('Bottom Layer') query to target objects (including objects on the Multi-Layer layer) that have shapes on the Top Layer or Bottom Layer.
QDrives , 04-12-2024, 03:53 PM
"Yes, outter layer has bigger minimal annular ring because of large drill value" -- No, usually it is more due to drift that the inner pads (annular ring) need to be bigger. The drill size does not matter that much."And is there rule to set minimal annular ring depending on layer copper height defined in stackup?" -- No, but you set it per layer if you want."Note that objects placed on the Multi-Layer layer will not be returned by the OnOutside query keyword" -- Ah yes. Only idiots work at Altium. As if a via is not present on outer/inner layers."ExistsOnLayer('Top Layer') Or ExistsOnLayer('Bottom Layer') " -- That is the correct query.
Use our interactive
Discord forum to reply or ask new questions.