Protel : microwave circuit layout tips

prev: protel_customize.htm -- next: ../pwb_layers.htm

Microwave circuits are much more sensitive to layer stackup than slower circuits.

• See ../io/rfs.htm for some useful books about RF circuit design.
• Tom Luttrell (2001) wrote a spiral generator in Client Basic to draw spirals in Protel using arc quadrants. You can get the latest version from http://groups.yahoo.com/group/protel-users/files/ then use the Macro:RunMacro process assigned to a menu item or toolbutton to launch.
• Brian Guralnick has written some utilities to generate interesting shapes:
  SpiralGeneratorProtelScript.bas -> smooth spirals
  InductorGeneratorProtelScript.bas -> Generates 'S' shaped printed inductors with rounded corners.
  SmoothTrackSizeTransitionProtelScript.bas -> Generates a smooth size track transition from size a-b at length c...
  ftp://ftp.point-lab.com/quartus/Public/ProtelUsers/
• spiral generator now with pick center and layer selection: Darren Moore on 2001-06-20 improved Brian Guralnick's code and posted it at http://groups.yahoo.com/group/protel-users/files/SpiralGen20.zip ``Note that you *must* install the new server that Ian Wilson was so kind to make for us all. This server is on the Yahoo groups site and also Ian's site http://www.considered.com.au/ExposePCBToMacro_V1_0.zip . I copied the following files to 'C:\Protel99\System' directory: ExposePCBToMacro.dll ExposePCBToMacro.ins ExposePCBToMacro.hlp Then install the server as per the readme file included''
• Abd ul-Rahman Lomax on 2001-02-01 01:56:47 PM explained:

  Subject:	RE: [PROTEL EDA USERS]:  Importing Gerber or DXF files
  
  At 08:20 AM 2/1/01 -0800, Pollock, Bryan wrote:
  
  >I'm trying to do a microwave circuit with more complicated shapes. I created
  >the spape I want in Cadkey and export it out in DXF. I can import it into
  >Protel and it works fine. I want to fill the shape and turn it into copper
  ...
  Depending on the frequencies involved, you may need high accuracy, better
  than one mil, so be careful in going through gerber, if you go that way
  that the resolution is at least 4 place.
  
  Since you have the shape in Protel from Cadkey, I assume that this shape is
  a set of line segments of line of zero width, or if there is a non-zero
  width, the centerline of the lines is the desired outline. I'll assume that
  the outline is also on the desired layer for the fill. If it is not, make
  it so. Highlight it; this will make it easy to delete.
  
  Oh, yes, do this on a scratch PCB, it will be a little easier. Set up a
  design rule for .003 mil clearance, board scope (3 microinches). Don't ask. :-)
  
  Now place a polygon fill, using Protel's snap feature
  (Design/Board_Options/Electrical Grid)
  ...
  to snap to the end of each line segment in sequence. Set up the
  polygon for a 0 grid (this causes efficient fill) and horizontal or
  vertical fill, whichever you think will be more efficient. Hatching is
  probably not necessary. Set the track width at 10 mils, I'd suggest. This
  board has no nets at this point. Be sure to uncheck "remove dead copper"
  and "pour over same net." When you are to the last segment, rt-click or Esc
  and the polygon will fill.
  
  Edit/Clear that outline.
  
  Corners will be rounded because lines always have round ends in Protel. If
  you want a square corner, place a fill. For other angles than 90 degrees,
  one may use a fine line, such as 1 mil, just at the corners, to sharpen
  them up. But usually if the angle is greater than 90 degrees it will be
  okay with nothing, or with a fill to sharpen up the corner. Or one may edit
  the polygon to have a finer line fill.
  
  The polygon, once it is complete, can be reduced to primitives
  (Tools/Convert/Explode Polygon...), and these can be copied and pasted into
  your footprint. It may help if, before you copy it, you place some pads in
  it to make it easy to pick up and while keeping it on grid, since the lines
  will be at some weird deviation from grid.
  
  Note that virtual shorts (fills, in this case, with a gap well under
  manufacturing limits, such as .002 mil, with an associated design rule that
  allows that specific clearance -- make the rule larger, say .005 mil) can
  be used to keep the two sides of the pattern distinct, so you can really
  treat this pattern, with pads placed at either end, as a component for
  schematic purposes, like any inductor or whatever.
  
  Okay, why .003 mils instead of .001 or 0. Well, Protel is little flaky
  below 10 microinches. Below 3 microinches, the polygon simply does not
  fill. Also, the actual gap with a 3 microinch setting, I found to be about
  8 microinches.
  
  
  Abd ul-Rahman Lomax
  LOMAX DESIGN ASSOCIATES
  PCB design, consulting, and training
  Protel EDA brokering (resale) services
  Sonoma, California, USA
  (707) 939-7021, efax (419) 730-4777
  
  ...
  *  Visit http://www.techservinc.com/protelusers/subscrib.html
  *  to unsubscribe or to subscribe a new email address.
  ...
  

end http://massmind.org/techref/app/protel_microwave.htm

Questions:

• -Remove-mirigoyen1 at spamcomcast.net asks:

  Hello,
  
  
  
  I am a user of Altium Designer (W09), involved with Flex and Rigid-Flex designs. I am looking for a way to customize or augment the Teardrop feature in PCB layout. I would like to be able to adjust the length and width of the teardrop segment(s). Does anyone know of a way, (besides manually adjusting each one) perhaps with a script?
  
  Kind regards,
  Mario Irigoyen
  

  +