prev: protel_customize.htm -- next: ../pwb_layers.htm
Microwave circuits are much more sensitive to layer stackup than slower circuits.
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:
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