Could you please help to set the Drill hole to Plane spacing in Xpedition VX2.6? Currently, Drill to Plane is applying the spacing of Pad to Plane.
Besides Pad-Plane clearance, you can define general Mounting Hole/Contour to Plane clearance following this:
1: Go Planes -> Plane Classes and Parameters
2: Select the Plane Class you want to apply this rule
3: Switch to Clearances / Discard / Negative Tab
4: Put desired clearance value into Mounting Hole/Contour clearance box (in Default Clearances area)
Thanks for your feedback. I tried to follow your guideline, but it is not help. For example, I want to set the PAD to Plane spacing is 12 mil, but the spacing of Drill to Plane is 9 mil. And I used suppress unconnected pad option.
You can add extra clearance on holes with no pads in general clearances:
Edit → clearances → general clearances → Additional * Hole conductor clearance
It is not work, because I can not set minus value (-3) on "Additional hole conductor clearance as you said.
As I know there's no direct way to achieve the result through clearance settings.
You should remove those pads that you are not using at the moment following those steps:
1: Open Padstack Processor (Edit -> Modify -> Padstack Processor)
2: On Pads tab, select Action: Delete, Select internal layers.
3: While keeping Padstack Procesor open, Select all vias you want to edit (you can use Find dialog to select all desired padstacks)
4: Return back to Padstack Processor. Select your via pad in the list, then press Process Pads.
5: This will remove all internal unconnected pads from via pads.
6: You can reset this result by selecting Reset action on Padstacks tab.
Hope it helps.
Thanks for your quick feedback, I could remove internal unconnected pads from via pads. But I still can not set the spacing rule as required.
Spacing from Drill to Plane (9mil)
Spacing from via Pad to Plane (12 mil).
Thanks a lot.
I believe there's no simple method to do that. I suggest you to set your minimum spacing (9 mils) to the Via-Plane and Pad-Plane and use ShapeEdit(in smart utilities) tool before finishing up. This way you can create static obstructs in your plane shapes with given offset to selected pads.
i suggest to use an route obstruct for every non plated mounting hole!
Retrieving data ...