Stats

  • Locked Locked
  • Replies 22
  • Subscribers 163
  • Views 28394
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Trouble with mounting holes and connectivity to shapes

EvanShultz
We used to use simple plated through holes for screw mounting, but a DFM review caused to us pre-emptively remove through hole barrels from under screw heads for fear of crushing the barrels. Our new mounting holes have 4 through holes outside of the screw head. There is an exposed copper ring, a shape, with both top and bottom Clines poking out of the copper ring to the through holes. To make life easy, we use a single pin with 3 vias (pin is in lower left of these screenshots), so engineers only have to make one connection on the schematic.

Although connectivity can't be assigned in the symbol, we noticed that dropping down the symbol in an unused area of the PCB assigned all copper and the vias to the net of the pin (gnd_sig2). Notice no DRC errors and all copper elements are properly connected together. [1.png]

I'll first plop this symbol onto a board with a shape on the bottom layer (green) assigned to gnd_sig1. As you can see, the vias decide to forget about the pin's net assignment and they get connected to the shape. The Clines touching the vias switch to gnd_sig1 as well, along with the copper ring on the bottom (green). You can see that the copper ring has voided around the pin's Cline, which is still connected to gnd_sig2. The copper ring on the top (red) also stays connected to gnd_sig2, so it doesn't void, but it creates DRC errors with the Clines on the vias which are now gnd_sig1. If I move the symbol off the shape, the vias report no net connectivity. [2.png, below]

Next, I'll drop the same symbol onto the same shape, but moved to an inner etch layer (blue, also set as TYPE=CONDUCTOR) and still assigned to gnd_sig1. This time, the copper ring on the bottom (green) doesn't void but the vias (and Clines) again attach to the shape while the pin is left unconnected as it's still assigned to gnd_sig2. DRC errors are again created. [3.png, below]

Finally, I'll drop the symbol down all alone and then extend the same inner layer etch shape (blue) to cover the symbol. You can see the vias aren't connected to the shape as they, and all other copper elements, retain gnd_sig2 attachment. This is how I'd expect it to always work. [4.png, below]

So, I've noticed different behavior if the shape exists before placing the symbol, than if the shape is added after the symbol is placed. Ideally, the net would be "fixed" to all elements with connectivity to the pin, in other words the only element with net connectivity (the pin) should drive connectivity to the rest of the symbol's elements, but that doesn't seem to be the case.

Adding a Cline arc that touches the Cline "spokes" would probably fix this, or changing the copper ring to a thick Cline arc, but before I change anything I'd like to get your feedback. Are our mounting hole symbols poorly designed for other reasons? Can we do something better? Is there a better fix than what I just proposed? Are we not properly using the SPB tools, which causes this issue? What do you guys do?

Thanks!

1.png
  • EvanShultz
    Here's a method to create the arcuate slivers shown in the screenshot above, courtesy of Mike

    Break up the shape by voiding lines:
    a. Define the initial shape (circle) on etch/top, with the size being the outer edge of the route keepout.
    b. Create another circle with the diameter being the desired width of the route keepout arcs, but the voiding backoff. I used 10mil smaller diameter circles, with a 5mil backoff, giving 5mil wide arcs.
    c. Define an "X" through the shape using “Add > Line”. (Using Clines sometimes does not void because they attach to the shape.)
    d. Select the shape, open up the Shape Parameters and change the “Suppress shape less than” to 0.000
    e. Go into Void Element (“Shape > Manual Void > Element”) and selects the outer shape to break it into 4 thin arcs. (Select “Void All” from the Right Mouse Button menu to do it quickly.)
    f. Use Z-Copy Shape ("Edit > Z-Copy Shape") to copy the resulting arcs to route keepout/all. Delete the unneeded elements on etch/top.

    However, I'm still left with the issue that copper on inner layers can sneak under the top and bottom shapes that are part of the symbol, inside the route keepout/all slivers, and create an island under the screw head. The island will connect to the 4 pins if the mounting hole has connectivity to that net, and the other islands aren't connected to anything so they can be deleted or ignored.

    It's perhaps not perfect, but this seems acceptable. Much better than before. Except that every sch mounting hole part has to be re-placed due to the pin number changing from 1 to 4. Yuck! But... maybe this is an example of "no pain, no gain". Anyone out there have any thoughts where potential problems may lurk?
  • mcatramb91

    Evan,

    A couple final notes:

    The Route Keepout arcs should be as close as possible to the 4 outside pins to prevent anything from routing around them.

    A special Anti-Pad should be used for the center non-plated hole to prevent any copper from ending up under the mounting hole compression zone. See attached image.   On the plane layers that the 4 outside pins don't connect to the anti-pad voids for the pins will fill notches in the center non-plated hole Anti-Pad and on planes the 4 outside pins connect you will have a direct connect so the shape can flow to the 4 outside pins. 

    If you are using dynamic shapes you may end up with isolated copper islands under the mounting hole that can be easily removed using Delete Islands (Shape > Delete Islands.)

    I worked out this solution several years ago for my past company and even though it takes a little extra work to generate these specialized shapes it makes the solution bullet proof and achieves the goal.

    Regards,
    Mike Catrambone
    Plexus Engineering Solutions

     

  • EvanShultz
    Hi Mike,

    Yeah, I figured out that the arcs need to be close to the pins and copper shape.

    OK, I see about the Antipad. And since the Antipad will be on all internal layers, as defined in the padstack, this works regardless of the number of layers in the board file. Very cool.

    Thanks again Mike!
  • EvanShultz
    Hi again Mike,

    I defined the Antipads using Pad_Designer to be larger than the drill hole, and then checked "Enable Antipads as Route Keepouts (ARK)" on the Parameters tab, to prevent any dynamic shapes from depositing islands between the copper rings on the top and bottom, that are part of the footprint. But that creates "Mechanical Pin Antipad to Shape Spacing" DRC errors where the antipad is over/under the copper shapes, since the ARK is for all layers.

    Alternatively, if the if I disable ARK, dynamic copper isn't prevented from leeching underneath the copper rings of the mounting hole footprint.

    Can you please provide more detail on the antipad?
  • mcatramb91

    Hello Evan,
    Sorry for the delayed response - busy week at work.

    I spent a little time this weekend generating a database demonstrating the solution for the mounting hole.  I created the mounting hole symbol from scratch and it only took about 15 minutes to complete.  I also created database with an 8 layer stackup with the mounting hole placed with two positive planes, two negative planes and two internal signal layers.

    I have film records created for each of the etch layers, generate gerbers and loaded them onto an additional film records for a side by side comparison.  Please take a look at the database and let me know what you think and if you have any questions let me know.

    I originally created the database in Allegro 16.3 and downrev'd it to Allegro 16.2 just in case you haven't made the move to 16.3 yet.  See attached ZIP file.

    Any question please let me know,
    Mike Catrambone
    Plexus Engineering Solutions

    Mike_Catrambone_Mnt_Hole_16_2.zip
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.