Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 10 replies
  • Answers 4 answers
  • Subscribers 93 subscribers
  • Views 4014 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

Selective thermal relief for thru holes, smt pads, vias in CircuitStudio?

nszmnsky

I often need to change the connection of a polygon depending on what connecting to - for instance, often want direct for vias but X on smt pads. Can this be done in CS? I don't see a way to configure rule for anything other than net, no option for setting what its connecting to.

 

Thanks

Neil

Parents
  • 0

    The answer to this question using the built in CS tools is no.  Altium have removed some of the query stuff necessary from AD.  They made a mess of this in my opinion.

     

    However, given this is tool I bought and use, I needed to find a way.  So I manually edit rules outside of CS and re-import them, as the backend is still the same as AD and still works the same way.  See my question over at the eevblog forum for how I do it:

    http://www.eevblog.com/forum/altium/polygon-pour-connection-for-vias/

     

    As an example, below is the contents of the exported and modified .RUL file for no relief on vias, but relief on everything else:

     

    SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|RULEKIND=PolygonConnect|NETSCOPE=AnyNet|LAYERKIND=SameLayer|SCOPE1EXPRESSION=IsVia|SCOPE2EXPRESSION=All|NAME=PolygonConnect_Via|ENABLED=TRUE|PRIORITY=1|COMMENT= |UNIQUEID=YEEDPGAH|DEFINEDBYLOGICALDOCUMENT=FALSE|CONNECTSTYLE=Direct|RELIEFCONDUCTORWIDTH=10mil|RELIEFENTRIES=4|POLYGONRELIEFANGLE=90 Angle|AIRGAPWIDTH=10mil¶

    SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|RULEKIND=PolygonConnect|NETSCOPE=AnyNet|LAYERKIND=SameLayer|SCOPE1EXPRESSION=All|SCOPE2EXPRESSION=All|NAME=PolygonConnect_all|ENABLED=TRUE|PRIORITY=2|COMMENT= |UNIQUEID=IPIHNEGD|DEFINEDBYLOGICALDOCUMENT=FALSE|CONNECTSTYLE=Relief|RELIEFCONDUCTORWIDTH=10mil|RELIEFENTRIES=4|POLYGONRELIEFANGLE=45 Angle|AIRGAPWIDTH=10mil¶

Reply
  • 0

    The answer to this question using the built in CS tools is no.  Altium have removed some of the query stuff necessary from AD.  They made a mess of this in my opinion.

     

    However, given this is tool I bought and use, I needed to find a way.  So I manually edit rules outside of CS and re-import them, as the backend is still the same as AD and still works the same way.  See my question over at the eevblog forum for how I do it:

    http://www.eevblog.com/forum/altium/polygon-pour-connection-for-vias/

     

    As an example, below is the contents of the exported and modified .RUL file for no relief on vias, but relief on everything else:

     

    SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|RULEKIND=PolygonConnect|NETSCOPE=AnyNet|LAYERKIND=SameLayer|SCOPE1EXPRESSION=IsVia|SCOPE2EXPRESSION=All|NAME=PolygonConnect_Via|ENABLED=TRUE|PRIORITY=1|COMMENT= |UNIQUEID=YEEDPGAH|DEFINEDBYLOGICALDOCUMENT=FALSE|CONNECTSTYLE=Direct|RELIEFCONDUCTORWIDTH=10mil|RELIEFENTRIES=4|POLYGONRELIEFANGLE=90 Angle|AIRGAPWIDTH=10mil¶

    SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|RULEKIND=PolygonConnect|NETSCOPE=AnyNet|LAYERKIND=SameLayer|SCOPE1EXPRESSION=All|SCOPE2EXPRESSION=All|NAME=PolygonConnect_all|ENABLED=TRUE|PRIORITY=2|COMMENT= |UNIQUEID=IPIHNEGD|DEFINEDBYLOGICALDOCUMENT=FALSE|CONNECTSTYLE=Relief|RELIEFCONDUCTORWIDTH=10mil|RELIEFENTRIES=4|POLYGONRELIEFANGLE=45 Angle|AIRGAPWIDTH=10mil¶

Children
  • 0 in reply to harvie256

    Thanks harvie256! IF I had a list of design rule options AND IF I wanted to manually create the rules I could accomplish what I need. I still have trouble wrapping my head around the use of rules to control PCB layout. I'm coming from NI Ultiboard where things such as reliefs, min width and spacing are Properties of the item, and each instance of the item can be individually manipulated. Want only one via direct connected? Just click on it and set the property. Want to set the relief style, spoke, and air gap of a polygon? Just click on it and set all those properties in one place. Problem is I haven't upgrade Ultiboard for a few years so have been evaluating other PCB packages to see if I should switch. I do like CS's ability to import from other PCB packages like Eagle as well as from Designer (by exporting as previous version). Of the PCB packages I've looked at, CS has the most plus's  - just not sure enough of them.

  • 0 in reply to harvie256

    As harvie256 said, they removed some helpful things, but the underlaying engine is still there. Same fate for concepts like object classes like net classes or component classes. I hope, altium reconsider this and bring this tools back in release 2.0.