Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 8 replies
  • Answers 1 answer
  • Subscribers 87 subscribers
  • Views 2946 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 change the default settings for vias?

batuu

Following the online documentation there are two possibilities to place vias.

 

1.) Press * key or Shift+Ctrl+Mouse wheel in interactive routing mode. You can choose the favorite via size in the Favorite Interactive Via Sizes dialog pressing Shift+V while routing.

2.) Press V to place a via when not routing. As the documentation says, a default via will be placed.

 

How do I change the default via settings? When nailing vias into polygons and planes, I am not in interactive routing mode and I do not want to change the settings for every via pressing the TAB key. I also do not want to select all vias with a filter and change the settings afterwards.

 

Oliver

  • 0

    Hi Oliver,

     

    I'll have the developers look at this and see if we can get a response.

     

    Tony

  • 0

    Hi Oliver,

     

    From the developers: 

     

    -- Tony

     

    The default settings can not be set in the interface of CircuitStudio, however the settings file may be edited manually. This requires a text editor that doesn't add any formatting to the file.

     

    Locate the file named ADVPCB.DFT in the following folder, with a name similar to:

    C:\Users\(WINDOWS USER)\AppData\Roaming\Altium\CircuitStudio {XXXXXXXX-XXXX-XXXX-XXXX-XXXXXXXXXXXX}

    (A shortcut to locating this is to use %APPDATA%\Altium\ in Windows Explorer).

     

    Please Quit CircuitStudio and then back up the file, in case it is damaged during the editing process.

    Open ADVPCB.DFT in a text editor and locate the lines starting with:

    RECORD=Pad|

    RECORD=Via|

     

    Then look along the length of the line to locate the settings to edit. For example, the XSIZE and YSIZE are in Pads and the DIAMETER and HOLESIZE are in the Vias.

    The settings are all stored in imperial (mil, i.e. 1000th of an Inch), even if your board is in Metric.

     

    See the example screenshot to see that the settings have been edited to:

    Pad:

    XSIZE=33mil|YSIZE=44mil

    Via:

    DIAMETER=31mil|HOLESIZE=21mil

     

    And see the metric Equivalent displayed in the Pad dialog. The Pad dialog has a Shortcut key Ctrl+Q to toggle the units between Imperial and Metric, which is useful if your board is in Metric but you want to calculate the values to store into the ADVPCB.DFT file.

     

    cz_LsiMXSr5OVdacwqEsg8

  • 0 in reply to e14softwareteam

    Hi Tony,

     

    thank you for this workaround. I will try it this way.

     

    In general, CS feels incomplete and we have workarounds like this (editing files in a text editor) for some workflows.

     

    Do issues like this become development tickets for the next releases?

     

    Is asking questions on this platform the best way to give feedback or to "open tickets"?

     

    Thanks, so far

    Oliver

  • 0 in reply to batuu

    Oliver,

     

    Thanks for the feedback.  CS is an evolving product.  The development team at Altium is highly committed addressing problems like this as quickly as possible.  v1.3 is scheduled to be released shortly and plans are already in place for a release following this.  In general each issue is flagged as a ticket and prioritized for future development.  This platform is an excellent avenue to flag issues like this.  Your also welcome to contact us directly at software@element14.com.   What most important is that we hear from users on their experience with CS so continue to provide feedback as you use the product!

     

    Tony

  • 0 in reply to e14softwareteam

    Sorry but how can this be the solution for a professional pcb design tool?

  • 0

    Just FYI, I find this annoying.  Along with the inability to turn off the soldermask using this method.  If I change the setting: SOLDERMASKEXPANSIONMODE=Rule to SOLDERMASKEXPANSIONMODE=None, CS just sets it right back to Rule.  There is no way to setup tenting by default.  If I try to copy and paste a via, it does not keep the Net that the copied via was attached to, and requires manually editing the net.

     

    So glad to see that "The development team at Altium is highly committed addressing problems like this as quickly as possible."  Here we are in 2019, v1.5.2, and this simple problem is not fixed?

  • 0 in reply to _aw

    The tenting property does seem to persist. If the tick boxes for "Force complete tenting on top/bottom" are checked these parameters copy and paste. Also when placing a via hit TAB to check the property of these check boxes and then any subsequent vias should maintain the same selection. The net assignment is lost during copy/paste but the TAB property change does work - set the net for the first via and then subsequent ones placed will keep the same net. If you have vias without nets then you don't need to change the net on each one individually - use the object inspector to change all selected vias.

  • 0 in reply to e14softwareuk

    That IS helpful Peter.  Thank you.  Hitting TAB before placing vias allows me to set it just the way I need it for all subsequently placed vias.  I just wish the user interface let you know about these secrets before you get frustrated trying to find solutions.  I guess if I would have read the F1 help page carefully, I might have realized that I could do this.