High Voltage - Explicit Design Rules

Outer Layer Rule "HV to LV :

For Designs with NO Inner Layer Vias (uVias or Buried Vias)

Example:  For Designs with Only Thru-Hole and Blind Vias use this Outer Layer Rule .

Scope1 Expression

InNetClass('HV') And Not OnMid

Scope2 Expression

InNetClass('LV') And Not OnMid

For Designs with Inner Layer Vias use ExistsOnLayer in your Scope.

Scope1 Expression

InNetClass('HV') And (ExistsOnLayer('Top Layer') Or ExistsOnLayer('Bottom Layer'))

Scope2 Expression

InNetClass('LV') And (ExistsOnLayer('Top Layer') Or ExistsOnLayer('Bottom Layer'))  

MId Layer Rule HV to LV :

Scope1 Expression

InNetClass('HV') And (OnMid or OnMultiLayer) 

Scope2 Expression

InNetClass('LV') And (OnMid or OnMultiLayer) 

Notes:

When using ExistsOnLayer the Top Layer and Bottom layer names must match the user defined long layer names in the stackup.

As of AD25 and older versions ExistsOnLayer is the only reliable solution for designs  with Inner Layer Vias (Stacked uVias or Buried Vias) that use clearance and creepage rules.  Skip Vias are also affected.

Tips: Best Practice when using ExistsOnLayer 

For designs using ExistsOnLayer in the Stackup Designer always use Altium's default long layer names Top Layer and Bottom Layer.

Why ?  Because the design rules will be broken if the layer count or layer names change.

Bad Practice

Good Practice

Outer Layer Rules Must Have Higher Priority

That's it !

Re-use Methods

Eric Albach

I just found a snippet design re-use method that is quite reasonable. Basically, append a question mark to the designators and create the snippets. Place the snippets in the new schamatic and PCB. Link the components between the schematic and PCB. Use Annotate Schematics Quietly. Update the PCB.

It's pretty easy. With this method it takes less than a minute to add a fully linked and annotated design. I used to spend a lot more time.

From the original schematic and PCB:
Update and Link the components between the schematic and PCB
Select the schematic section

Use SCH Inspector set to include only parts and use Smart Edit Formula on designators to append with a question mark.
        
Example formula : !+'?'

ends up with R12? (leaving the numbers keeps the components linkable and the question mark allows quiet annotation)

Update the PCB with the new designators
Create the schematic and PCB snippets

In the new schematic and PCB:
Place the snippets
Link the components using Project > Component Links > Add Pairs Matched by Designator
Use Annotate Schematics Quietly
Update the PCB

Source https://forum.live.altium.com/posts/221757/645999

Rich Betz

When you paste PCB snippets, be careful with existing 'ON' Planes. Your via's can and will connect to the first plane they contact, throwing your net connections all out of whack.

Either turn off all of your Plane Layers before you place the snippet, or place it outside the board outline until you get all of your component net connections linked up correctly.

When you get your Sch/Pcb component pin nets all linked up with All Layers On, select the whole snippet area.

Use PCB Filter (IsSelected and (IsVia or IsTrack))  to filter out the parts but hold on to all the connections.

Then CUT the connections with reference to Pin1 somewhere in the snippet,

Then Paste right back in the same place.  All tracks and via's will adopt NetName from component pin nets.

Then... you can turn your Planes back on and position the snippet where you want it.

Source: https://forum.live.altium.com/posts/221757/646088

Eric Albach 

Possibly the best method for the PCB side is to keep "snippets" in a PcbDoc then you can select, copy and paste special with Keep Net Name. That way you won't lose the polygon pour nets.

Source: https://forum.live.altium.com/posts/221757/646099

TrueType Fonts in PDFs

Workaround:

"Open the file in real adobe acrobat or the viewer rotate the pages and then rotate them back and then save. Files can now be saved. Doing this probably removes the bug that Thomas mentions and puts it back to the correct standard."


Source: Altium Ideas

Delphi File Basics

function Read_ini(junk:string):boolean;

var
  folderName : string;
  fileName : string;
  myFile   : TextFile;
  data     : string;
begin

     //showmessage (Board.FileName);
     //showmessage (PCBServer.GetCurrentPCBBoard.FileName);
     //showmessage (ExtractFilePath(Application.ExeName));
     //showmessage (ClientAPI_SpecialFolder_AltiumApplicationData);

     // For ini file Saved in Project Folder
     FileName := (ExtractFilePath(Board.FileName))+ 'Designators.ini';

     // Global ini file
     if Not FileExists(FileName) then
     begin
       // Try to open a text file for writing to
       folderName := ExtractFilePath(ClientAPI_SpecialFolder_AltiumApplicationData) + 'Scripts\';
       CreateDir (folderName);
       FileName := folderName + 'Designators.ini';
     end;

     //showmessage (FileName);

     if FileExists(fileName) then
     begin
         AssignFile(myFile, fileName);

         // Reopen the file in read mode
         Reset(myFile);

         // Read the file contents
         //while not Eof(myFile) do
         //begin

         //ShowMessage(data);

         if not Eof(myFile) then ReadLn(myFile, data);
            EditMinHeight.Text:= data;

         if not Eof(myFile) then ReadLn(myFile, data);
            EditMaxHeight.Text:= data;

         if not Eof(myFile) then ReadLn(myFile, data);
            EditCommentsTop.Text:= data;

         if not Eof(myFile) then ReadLn(myFile, data);
            EditCommentsBot.Text:= data;

         if not Eof(myFile) then ReadLn(myFile, data);
            EditTestPointsTop.Text:= data;

         if not Eof(myFile) then ReadLn(myFile, data);
            EditTestPointsBot.Text:= data;

         //end;

         CloseFile(myFile);
         result := True
     end;

     // Debug Code
     // Now see if the file exists
     // if FileExists(fileName)
     // then ShowMessage(fileName+' exists OK')
     // else ShowMessage(fileName+' does not exist');

     // Delete the file and look again
     // DeleteFile(fileName);
     // if FileExists(fileName)
     // then ShowMessage(fileName+' still exists!')
     // else ShowMessage(fileName+' no longer exists');

end;


function Write_ini(junk:string):boolean;

var
  folderName : string;
  fileName : string;
  myFile : TextFile;

begin

  // Open a text file for writing to

    // For .ini files Saved in Project Folder
    fileName := (ExtractFilePath(Board.FileName)) + 'Designators.ini';
    AssignFile(myFile, fileName);
    ReWrite(myFile);
      Write(myFile, EditMinHeight.Text + #13#10);
      Write(myFile, EditMaxHeight.Text + #13#10);
      Write(myFile, EditCommentsTop.Text + #13#10);
      Write(myFile, EditCommentsBot.Text + #13#10);
      Write(myFile, EditTestPointsTop.Text + #13#10);
      Write(myFile, EditTestPointsBot.Text + #13#10);
    CloseFile(myFile);

    // Global ini file
    if Not FileExists(fileName) then
    begin
      folderName := ExtractFilePath(ClientAPI_SpecialFolder_AltiumApplicationData) + 'Scripts\';
      CreateDir (folderName);
      fileName := folderName + 'Designators.ini';
      AssignFile(myFile, fileName);
      //DeleteFile(fileName);
      ReWrite(myFile);
      Write(myFile, EditMinHeight.Text + #13#10);
      Write(myFile, EditMaxHeight.Text + #13#10);
      Write(myFile, EditCommentsTop.Text + #13#10);
      Write(myFile, EditCommentsBot.Text + #13#10);
      Write(myFile, EditTestPointsTop.Text + #13#10);
      Write(myFile, EditTestPointsBot.Text + #13#10);
      CloseFile(myFile);
    end;

end;


Debug Code

     // See if the file exists
     // if FileExists(fileName)
     // then ShowMessage(fileName+' exists OK')
     // else ShowMessage(fileName+' does not exist');

     // Delete the file and look again
     // DeleteFile(fileName);
     // if FileExists(fileName)
     // then ShowMessage(fileName+' still exists!')

     // else ShowMessage(fileName+' no longer exists');

Related Links:
Delphi Basics : Files

Track Coordinates X1,Y1 and X2,Y2

In Altium Track Coordinates are in mils x 10,000

click on image to view

Notes:

X1 is always less than X2.

Y1 can be less than or greater than Y2, it depends on the angle of the track and the starting location of the X axis.

That's it !