We're now faced with the problem, that we need to add fiducials on the boards where we need to have a solder mask free area with a diameter of 3 mm and a copper pad of 1 mm in its center. Since the solder mark is defined for all pads on the board I have no idea how to solve that with Pulsonix.
Create Doc Symbol with a pad style of round 1.00 mm, then Edit Technology, select the pad style, and use By Layer to make the Solder Mask 3.00 mm for both Top and Bottom.
If you go over to the old Pulsonix Yahoo user group here:
Ben, thanks a lot for your advice. This is what I tried first, because this would be the way I get it done with the software used by us before we started with Pulsonix. But could not assign any shape I tried to be on the solder mask layer.
Thanks James, I did not solved it yet. I did not notice the "by layer" button and will play a bit around with it now.
Got it - followed the instructions given by Ben and finally I have a result we can work with. My problem was, that no solder mask layer exist when I edit the default fiducial - that's why I wasn't able to make the correct assignment.
I never expected that the default comes up with a single Top-layer only ! I really need to accustom myself to load a technology first instead of relying on the one which opens with the file I edit.
When you open an item from the Libraries dialogue, pre-select the Technology, you wish to open it up with. If no technology is chosen (None) then the system will default to a minimum set.
The IPC and SEMA standard for a PCB fiducial is a 1.00 mm diameter round pad with a 3.00 mm diameter clearance of copper and solder mask, as Xeint was wanting to put down.
The fiducials I uploaded to the old Yahoo Pulsonix group matched this IPC specification.
Local fiducials for fine pitch components differ. The PCB Libraries Footprint Expert outputs these:
Nominal: 0.75 mm round pad, 1.50 mm clearance of copper and solder mask. Least: 0.50 mm round pad, 1.00 mm clearance of copper and solder mask. Most: 1.00 mm round pad, 2.00 mm clearance of copper and solder mask.
I guess these will be in the IPC-7351C revision when it's released.
I find using a pad and the by layer feature neater than adding a drawn circle solder mask clearance. You can modify it more easier in the PCB layout by using Alternate Pad Style and editing the pad style where as you can't edit a drawn solder mask clearance.
It also offers the advantage of being easily modifyable at the CAM side in the gerber data if needed since both the copper and solder mask would translate to gerber as single apertures that could be adjusted whereas a drawn filled circle would remain as a drawn filled circle and bit more tiresome to adjust (it can be done but needs more clicks in the CAM tool).
This is in the event that the assembler needs to modify the fiducial for their process after they've contacted you of course for permission!
Posted - 06 Jan 2015 : 09:19:57
