The gateway to online resources and design support for engineers, powered by RS ComponentsAllied

+Post a new topic

Fiducial marks?

Avatar Posted by passpics at

Anyone have any tips for creating fiducial marks in DSPCB? Needs to be a component, so the PnP machine has the X-Y coordinates.

I've tried everything I can think of, but can't seem to get DSPCB to do this:

1/ 1.5mm diameter plain solder pad, no hole
2/ 3mm diameter area around the pad with no copper, solder mask, silk screen or anything else. Should act as a keep out for copper pour.

Any ideas anyone?

Thanks,
Martin

Replies

  • Avatar

    Posted by Boss at

    Fiducial Lib Comp.zip
    (1.26 KiB) Downloaded 2 times
    Assuming you only need a copper pad without a hole.

    You can go into the Design Technology File Shift+T and create another style "add style" on Pads tab.
    Give it the name Fiducial and the diameter you want, set hole to zero and untick plated.

    Or you could create a PCB only component in the Library Manager.
    Select surface mount pad and change to "round" of the size you require.
    My attempt attached.

    I couldn't find a way of setting the solder resist spacing for this pad.

    Let us know if that helps?

  • Avatar

    Posted by passpics at

    Thanks Boss. As you say, seems like no way to adjust the solder mask. It's supposed to look like this:

    Round_fiducial_on_pcb.jpg
    Round_fiducial_on_pcb.jpg (32.83 KiB) Viewed 909 times


    For now I'm using a pad like your example, and manually adding a round copper pour keep out, but still see no way to adjust the mask... This is such a standard thing, I'm sure there must be a way?

    Cheers,
    Martin

  • Avatar

    Posted by passpics at

    Ahh, found how to modify the solder mask :- Just add a new "Solder Mask" layer to the Design Tech file when editing the fiducial mark component, and draw a filled circle on that layer. Have not output the plot yet, but looks like it will work.

    Still can't see a way to add a copper pour keep out to a component, but I'll manually add that for now on the PCB. This is good enough.

  • Avatar

    Posted by Boss at

    Hi Martin,

    Yes agree, I continued experimenting and did the same with my component after seeing this old post on the Forum

    Posted by gx at Mon Oct 10, 2011 1:01 pm
    I found a way of adding the solder mask layer in design technolgy :)
    I coloured it pink and moved it down the list so it was below the top tracks red layer so theyre both visible


    Perhaps you could share your component on the Forum for others when checked?

  • Avatar

    Posted by Boss at

    Possible solution....

    Create the fudicial SM pad as before, but then create a second pad of type "Annulus".
    Set this for say 3mm width and inside of 2.8mm, turn hole off (set to zero) untick plated. This represents the isolation ring so will act as a keep out.
    Create your solder resist layer.

    From experience you need to create the two pads side by side and when both are the correct size (check track width of annulus) place one over the other to make concentric. (Working on them in their concentric locations causes selection problems).

    Save as PCB symbol and then produce the library component.

    Fiducial.jpg
    Fiducial.jpg (32.13 KiB) Viewed 872 times

  • Avatar

    Posted by Boss at

    Hi, here is my Fiducial component set for 3mm
    The solder resist is automatically taken care of by the footprint of the annulus which should also act as a 'keep out' for any copper pour.

    Fiducial3mm.zip
    (2.25 KiB) Downloaded 7 times

  • Avatar

    Posted by passpics at

    Thanks Boss! Excellent idea, don't know why I never thought of using a pad within a pad. Problem solved.

    Regards,
    Martin

  • Avatar

    Posted by wenmor at

    Thanks BOSS for the component. Downloaded it and works very well for the solder mask and copper area 'keepout'
    The only downside I found is the Pad to Pad DRC error because 2 pads on top of each other or am I missing something here?

    It would be very nice to be able to specify a clearance for pads in a future revision

    regards
    Tony

  • Avatar

    Posted by Boss at

    Hi Tony,

    Thanks for the feedback. No you are not missing anything, I thought DRC would throw up an error, but remember it is just a "Check", so if you are happy with what is pointed out, it can be safely ignored.

Post a reply