Stats

More Content

Issue with Via-Via Constraints

WG20250730781

Hi all, 

I have an issue with the via-via constraints of my design.

1. Normally, the via-via distance is defined in the constraints manager. However, the thru via to thru via spacing is defined by the air gap between the two vias. The issue is that this air gap accounts for the pad size to pad size distance of the via, and not the hole-to-hole distance itself. Often in manufacturing, hole-to-hole distance is more important in fabrication. How do I account for actual hole-to hole distance itself?

2. Under the constraints manager, there is a column that specifies 'hole to hole'. When I double click it, it pops up another window and further classifies into so many other line items:



However, under the general constraints manager window, there is already 'Thru via to Thru via'. How are these two different?

I appreciate some professional help.

Thank you.

Parents
  • +1

    Hi

    In Allegro there is the option to do Hole to Hole checking of various objects such as vias etc. Typically this analysis mode is not enabled in the constraint manager and would need to be enabled. To check that in the constraint manager go to Analyze > Analysis Mode. Under spacing you can check that "Hole To" is enabled for the various objects such as vias etc.

    The hole to hole spacing checks the distance between the edge of the hole barrel between holes in the board. If you do a search in the help file for Hole to Hole it explains what it does with a graphic as a visual cue.

    The main difference between this mode and  say standard via to via to via checking is that with standard via to via checking the drc is basically checking the space between the via pads and ignores the drill.

    This hole checking mode maybe tied to a certain license option in Allegro, not too sure. On the Orcad pro ver 17.2 x I have not had success in getting this rule to work. Perhaps someone can chime in on that and clarify.

    You could probably test it fairly easily on your vias by entering a value that exceeds any via to via spacing so as to see it is actually checking hole to hole spacing or not.

    Best Regards.

  • 0 in reply to excellon1

    If memory serves me correctly the hole to hole rules don't take affect unless the the pads are suppressed. You can set this up in Cross Section Editor, look at the Physical section. If you have this enabled then hole to rules will be used on holes that are exposed. This is available in all license levels but the higher you go up the more hole to options can be used. 

  • 0 in reply to steve

    Hi Steve & JC

    Yes indeed it works "Foggy Memory here :)"

    Just a quick explanation of a use case for this. On a multi Layer design with allegro it is possible to Suppres pads. This is useful on the inner layers where by the pad of a via can get removed visually and only the drill hole is left. Basically it means it is possible to create a tighter layout
    because a pad is removed. If a connection is made to the drill hole then the pad shows up.

    The hole checking DRC if enabled then comes into play to check the distance between the hole and an object such as a trace, via etc.

    To get this to work. Unused pads suppression and display padless holes should be checked in the cross-section editor & The hole checking DRC mode needs to be enabled in the constraint manager with suitable values for the actual drc spacing.

    Only thing to be aware of is if unused pad suppression is used on a multi-layer design and there is no physical connection to a padstack on those inner layers then the pad gets removed. This means that all that will exist is the barrel of the drill on that layer. If you prefer a physical pad to exist on a inner layer that has no physical connection then don't use suppressed pads. Depending on the design the pad on the inner layer can be used as a "Anchor for the drill hole" . There is a debate on this with respect to board reliability and having a pad as an anchor on inner layers.

    Thanks for the memory jog guys.

    All the best..

  • 0 in reply to excellon1

    Hi all, so what I'm getting from this discussion is this:
    - If I want to set up hole-to-hole constraints, then I need to enable pad suppression (only works for inner layers)
    - This will effectively remove all the pads that are unused and the hole-to-hole constraint will then take effect as I intended.
    - But all the pads will be removed (not intended).

    If the pads are still present, no matter what, it will ALWAYS override the hole-to-hole constraint.
    (Is this true? If so, then there is no physical way to set up hole-to-hole clearance WITHOUT removing the pad itself, right?)

Reply
  • 0 in reply to excellon1

    Hi all, so what I'm getting from this discussion is this:
    - If I want to set up hole-to-hole constraints, then I need to enable pad suppression (only works for inner layers)
    - This will effectively remove all the pads that are unused and the hole-to-hole constraint will then take effect as I intended.
    - But all the pads will be removed (not intended).

    If the pads are still present, no matter what, it will ALWAYS override the hole-to-hole constraint.
    (Is this true? If so, then there is no physical way to set up hole-to-hole clearance WITHOUT removing the pad itself, right?)

Children
No Data
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.