Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 5 replies
  • Subscribers 89 subscribers
  • Views 4464 views
  • Users 0 members are here
Related
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

Plane Clearance Around Component Pads

bills_alsentis

Greetings Again,

 

I have a line of pads I use for In Circuit Serial Programming for micro's that are spaced 2.54mm apart for use with a pogo pins/test probes fixture.  I added a Polygon Pour Plane (Gnd) to the same layer and would like to increase the pad to poly clearance around the pads to more than my default clearance of 0.2mm to prevent the pogo's from shorting to the plane with an unsteady hand - without having to increase the overall 0.2mm clearance for all the other components on the layer.

 

image

 

I originally looked at adding a keepout to this layer, but this will not work as a keepout over the pads obviously creates DR violations.

 

So I turned focus to creating a 2nd Power Plane Clearance Rule.  Since all 5 pads are the same size and unique to all other pads in my design, I created a Pad Class to include these pads and increased the Clearance.  Unfortunately this did not work as my default Clearance rule of 0.2mm was maintained after repour.  I then decided to make a 2nd Clearance Rule, but the "Where The First Object Matches" rule dialog does not include an option to select Pad Class like the Power Plane Clearance does.

 

I am relatively new to CS, so I must be missing something here.  I would have thought the original Power Plane Clearance would have worked - do I have to somehow label my plane as a "Power" plane or similar?  Is CS not recognizing it as a Power plane?  Might there be a way to create a rule for clearance around certain components?

 

I understand the Rules are executed based on Priorities, but I did not see where this was giving me the issue.

 

Any help to understand better is appreciated - Thanks

  • 0

    The fix for your clearance problem will require some text editing but I guarantee it will work.   The following are the steps that you need to take:

     

    1-Go into your PCB Rules and Constraints Editor (Right-click and select Design --> Rules)

    2-In the Clearance section of the rules, duplicate the Clearance rule.  Name it Clearance_pogo or something like that.

    3-Give it a higher priority than the original Clearance rule.

    4-Export the Clearance RUL file.  Sometimes this gives me problems.  Sometimes it exports.  Sometimes it doesn't.

    5-Open the RUL file with a text editor such as Notepad++.

    6-Look for your Clearance rule that you just created.  Around the middle of the line it will have "NAME=Clearance_pogo".  It should be in the same order as the order in which it was placed in CS.

    7-Find SCOPE1EXPRESSION=All.

    8-Change "All" to the following:

         HasFootprint('Pogo PAD')

         Except "Pogo PAD" will be the name of YOUR footprint.  If you need to know what it's called, double-click on the footprint in CS and you will see the Name of the Footprint.  Copy and Paste that name.

    9-Save the text file.

    10-Import the RUL file into CS as a Clearance rule.

    11-In the rules you will see that both scopes utilize "All" in the drop-down menus but this will not be the case.  Don't change these values.  Click on the Clearance Heading and you will see that the first scope shows "HasFootprint('Pogo PAD')"

    12-Repour your polygon.

    imageimage

    Extra-If you don't wish to utilize a clearance for a particular rule, you can just delete the number.  It should then use the following Clearance rule.  Here's a pic.

    image

    If you're wondering how I figured all of this out, I used to use Altium quite extensively.  A lot of these features are available in Altium but are limited in CS.  I used to do a lot of text editing of my Altium projects because it was limited in the functionality that I needed.  Luckily both CS and Altium are text-based.

  • 0 in reply to adamwebber

    Sweet!

     

    Thanks James, worked like a Champ - pretty confident I would have never figured that one out with the limited CS documentation out there.....

     

    Coming from many years in PCAD, the CS learning curve has been slow due to its non-intuitiveness; but just as in this case, I have been impressed with the capability of CS once a solution path is unearthed.

     

    Hope this helps other s in the future too - thanks again!

  • 0 in reply to adamwebber

    Actually this "manual" Clearance rule also helped with custom plane backoff from my fiducial pads as well....

  • 0 in reply to adamwebber

    Hi JC,

     

    You suggestion is good so I gave it a like.  I'd like to mention that there seems to be 'some' capability in CircuitStudio for defining advanced rules that gets to some of what you mention. If you open the PCB Rules and Constraints Editor, then launch the Rule Wizard feature, you can enter the name and comment and then choose the rule scope as Advanced.

    image

    In the next window it allows entry of conditions for scope.  There is partial query builder function from the AD tools here.  In the case mentioned, I could choose first condition as Exists on Layer and then Top Layer and the Query preview enters OnLayer('Top Layer').  Then I could add another condition, Belongs in Polygon and query preview fills in InNamedPolygon('***') with a drop down box that shows some of the polygons I have created and named.

    image

     

    After you generate a rule this way there doesn't seem to be a way to edit the scope through the GUI but you can do what you suggest and export to a text editor, update and then re-import.

     

    There is an older thread that has some related information.

    How to edit rule scope in Circuit Studio

     

    And, another related link about making a rule for direct connection of vias with thermal connection to pads.  This describes making a default rule that is direct connect and a higher priority rule that anything in the component class will be thermally connected.

     

    https://www.eevblog.com/forum/circuit-studio/how-to-selective-thermal-relief-for-vias-and-pads/

     

    It should be possible to make a rule that is more specific than described using the IsVia keyword.  Some of these keywords are described here: https://www.altium.com/documentation/altium-designer/pcb-queryobject-type-checks-ad and https://www.altium.com/documentation/altium-designer/query-language-reference-ad

    I'm not sure if CircuitStudio supports them all.

  • 0 in reply to adamwebber

    So glad I could help.  I don't really have a job anymore so I sit around monitoring the forum here looking for requests. image  Sometimes I can help.  Sometimes I need help.