I want to make remove unused pad/via at inner layer in order to increase area. But I wonder that does it cause problems in terms of IPC Class-III or PCB manufacturing?
Removal of unused inner via and throughhole pads is standard in PCB tools. You should be aware of drilled hole to copper spacing requirements that have still to be met. Minimal hole to copper clearance is considerably larger than copper to copper due to drill tolerances.
Another point is that you may want to keep inner pads of press-fit pad stacks.
Removal of unused inner via and throughhole pads is standard in PCB tools. You should be aware of drilled hole to copper spacing requirements that have still to be met. Minimal hole to copper clearance is considerably larger than copper to copper due to drill tolerances.
Another point is that you may want to keep inner pads of press-fit pad stacks.
Always remember a PTH hole is drilled 0.1mm larger than the finished hole diameter, so you need to add 0.15mm extra clearance around the hole. Do that and you will have no issues with class 3 designs, I have been doing it for 20 years...
So if std. design spacing is 0.2mm for unsupported PTH holes on inner layers it should be 0.35mm. Some software has a "drill oversize" function to cater for this, in those cases set drill oversize to +0.15mm and keep spacings the same.
What do you mean, if they are unused, there is no problem... The drill hole is still present and you have to cater for any inner layer track or copper pour to the hole at the size it is drilled. Which as stated is usually 0.1mm larger than the required finished hole dimension. I would suggest you do some studying of IPC standards and maybe look at IPC CID courses.
I have completed both the CID and CID+ courses...