Stats

  • Locked Locked
  • Replies 5
  • Subscribers 164
  • Views 4016
  • 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

Thermal Reliefs don't appear for thruholes

qwertyuser

Hello,
I'm using OrCAD 16.2's PCB editor to construct a simple board, mainly as a learning exercise. I wanted to create a thermal relief on a layer a plated through-hole passes through. The through hole belongs to a 6 pin connector, and it's suppose to touch the ground plane on pins 4 and 6 in the attached screenshot. However my padstack does not seem to be working, instead of there being an antipad a cross appears over the hole. Antipads are also not created for pins that should not be touching the ground plane pin 5 for example. Neither the thermal relief nor the antipad variables affect the layout at all, the only thing that seems to change anything in the layout is the regular pad variable.
The information dialog indicates that the blue plane is part of net 0 (which is correct).

The plane was laid as dynamic copper, and declared to be part of the ground net. When highlighting the ground plane, the correct pins light up but thermal reliefs just do not apper.

Screenshot

I've been struggling with this problem for the past 2 days, someone please help.

 

Edit: Here's another screenshot, the crosses that appear over the through holes should be thermal reliefs.

  • EvanShultz

     Hi qwerty,

    Are the crosses the thermal reliefs? It looks like you just might have your thermal reliefs set to Orthogonal.

    To see the thermal relief type, go the Shape > Select Shape or Void and pick the shape. Then choose Parameters from the RMB menu. On the last tab of the Shape Parameters form, Thermal relief connects, can you choose the type of thermal reliefs you want. Try changing the "Thru pins" type to "Diagonal" or "Full contact" and see what happens.

    It looks like the black ring between the pad and the shape is the clearance. You can adjust this from the Physical domain in Constraint Manager (CM). CM is a big tool so if you haven't looked into it yet, consult the manual and just play around with it to get a feel for CM.

    Is that what you're looking for? Did I misunderstand your question?

  • qwertyuser

    Thank you for replying. When I tried doing the "Select Shape or Void" on the connector shape itself I was unable to find "Thru pins" on the last tab. Sorry about constantly linking you to screenshots but I think they can explain my situation better.

    ( Screenshot  1 ) Here's what the Shape Parameter form of the connector looks like, the top instance of PCB editor shows a completed board file that was included with my book, and the instance on the bottom shows my attempts at recreating the example from scratch.

    ( Screenshot  2 ) This time I selected the shape of the plane and the last tab does show the "Thru pins" option, which I then changed to Diagonal. Initially though both Shape Parameter forms looked the same.

    I should mention that the thermal reliefs for both designs are defined as flash symbol "TR_180_150" in the padstack editor.

    My question basically is, how do I get my layout's thru holes to look like those of the design I'm trying to recreate (top instance)?

    Thanks again.

  • redwire

     Are you using negative or positive power planes?

  • qwertyuser

     I'm using positive power planes. I've been messing around with the constraint manager and by importing the working design's constraints I can get it to work, I just have to figure out which constaint it specifically is.

     

    EDIT: Making the planes negative fixed it. Thanks for hinting at that. I'm a little confused now as to why they're suppose to be negative layers.

  • redwire

    There's a lot buried in the user manuals -- you might search "negative planes" and see what hits you get.

    It seemed as though you were describing a thermal flash symbol which is only used with negative planes. Try removing the thermal flash symbol in the padstack if you're going to use positive.


    I do all of my designs with negative power planes....

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.