Actions
Forum Thread Details
  • State Not Answered
  • Locked Locked
  • Replies 6 replies
  • Subscribers 84 subscribers
  • Views 1612 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

How to make a component keepout that allows tracks?

bigbaldjohn

Hi,

I'm using CS 1.5.2.

I'm designing a PCB for a housing that has support pillars placed all over the PCB and need to be sure I don't place components in these areas. Tracks are OK.

If I put the contact areas onto the keep-out layer I can't put tracks there, which is not what I want.

I've tried putting a Fill onto Mechanical 15 layer (Courtyard Top), which is OK for eyeballing but I don't get a clearance violation in DRC.

I've added the following Clearance rule but it didn't help:

SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|UNIQUEID=RIRCENJA|

RULEKIND=ComponentClearance|NETSCOPE=AnyNet|LAYERKIND=SameLayer|

SCOPE1EXPRESSION=(OnLayer('Mechanical 15') OR OnLayer('Courtyard Top'))|

SCOPE2EXPRESSION=All|

NAME=ComponentClearance_Courtyard|

ENABLED=TRUE|PRIORITY=2|COMMENT= |DEFINEDBYLOGICALDOCUMENT=FALSE|

GAP=0mil|

COLLISIONCHECKMODE=3|VERTICALGAP=0mil|SHOWDISTANCES=FALSE¶

(all one line in the .RUL file)

 

What am I doing wrong please?

 

Cheers

John

Parents
  • 0

    It is a good question and it has come up before in the forum.  I found that if you use the rule wizard you can start to define a rule based on a selection of a named polygon.  However, if you try that the rule ends up showing as 'all'.  If you export the rule and look at the text in a text editor you will see the text SCOPE1EXPRESSION=(InNamedPolygon('MyNamedPolygon')  but it does not appear to be recognized in CircuitStudio.

     

    I have worked around this by placing 3D bodies where I want height restrictions.  You can define simple 3D bodies and place them as free models.

     

    Expanded rule capabilities are something CS badly needs to be a professional tool.

     

    Perhaps someone else has a solution?

     

    [I think in AD this is done by defining rules based on rooms that you place]

Reply
  • 0

    It is a good question and it has come up before in the forum.  I found that if you use the rule wizard you can start to define a rule based on a selection of a named polygon.  However, if you try that the rule ends up showing as 'all'.  If you export the rule and look at the text in a text editor you will see the text SCOPE1EXPRESSION=(InNamedPolygon('MyNamedPolygon')  but it does not appear to be recognized in CircuitStudio.

     

    I have worked around this by placing 3D bodies where I want height restrictions.  You can define simple 3D bodies and place them as free models.

     

    Expanded rule capabilities are something CS badly needs to be a professional tool.

     

    Perhaps someone else has a solution?

     

    [I think in AD this is done by defining rules based on rooms that you place]

Children
  • 0 in reply to tarribred61

    I tested this a bit more and found that the component clearance rule works sort of.  You can set one criteria to be a component class (for example top side components) and then the second criteria could be all.  Then any 3D body you bring within the horizontal or vertical clearance zone would cause a violation.  What this lacks is ability to define a zone to apply the rule.

     

    You can, perhaps, make that zone by making a section of the pillar as a mechanical component with a 3D body that you place on the PCB at the location you want to keep things out of.  Then the normal component clearance rule should work.

     

    If you need to, you might add a new component class that contains the mechanical component and then you could base a rule off that component class.  Then you could have special clearance rules that differ from the normal clearance cases.

     

    If you put the mechanical part on the PCB but not on the schematic, when you update the PCB it will likely want to remove the part on the PCB.  You can put a corresponding part on the schematic.  Its schematic symbol might just be a text box or something simple and the schematic part would call out a PCB footprint.  That footprint would have the 3D body (or enough of it to act as the keep out zone).

     

    This is then just like putting any other part on your board that you can route under.

  • 0 in reply to tarribred61

    Wow, thank you Thomas. I appreciate you spending the time, I'll experiment along the same lines.

     

    But what a faff for something that must be a fairly common requirement. Pity Altium aren't listening...