At 06:36 PM 6/13/01 -0400, Brian Guralnick wrote:
>I just tried to fool Protel into converting it's trace ends from arcs to
>squares by modifying an ASCII Protel file. Guess what happened, Protel
>converted the tracks to fills on load. Though it didn't do such a bad
>job, all 45 degree angle tracks were totally messed up. I guess this is
>why Protel does not offer the square end tracks in the first place.
I'm a little mystified here. "converting its trace ends from arcs to
squares by modifying an ASCII Protel file" does not explain to me how one
might even attempt to do this. Protel traces are, to my knowledge,
inherently created with round draws. Protel cannot properly import square
draws. As Mr. Guralnick seems to have discovered, it will attempt to
convert them into fills, which works when they are orthagonal and fails
miserably when they are not. Since it *does* import square track as fills,
I'd say it is a bug that it does not handle draws at angles other than 0 or
90 degrees.
That Protel does not support rectangular draws in the database is not a
bug, it is a missing feature. It would not be terribly difficult to add the
feature, I'd think. But it would only be used rarely. More useful, for
certain RF patterns, would be true polygons, with corner angles less than
90 degrees. At least I've had call for that from an RF engineer, and I had
to simulate it with 1 mil draws.
>About the Gerber import. For this same potential bug, Protel breaks up
>the lines into many elements though it does not have to.
??? If gerber lines are generated properly -- that is, in the Protel syntax
-- the gerber will import as-is, one segment per draw. If the gerber is
broken into too many elements, so will the Protel import.
> When making my SPIRAL.BAS, I discovered the Gerber pen up & pen down.
Kinda important...
> When importing my spirals, Protel broke them up into all the elements
> even though I properly controlled the pen from the beginning to the end.
I don't know what else would be expected. I assume that Mr. Guralnick
generated a series of X,Y coordinates. This will be interpreted, provided
that the "pen" is down (the "light" is on) at the beginning, as a series of
line segments. Two points will give one line segment, and each additional
point, if the light is kept on, will generate an additional segment, from
the last data point to the next. That's what gerber does, and so that is
what you get when Protel imports the gerber.
>I'm going try to make another mod to see what happens.
>
>_____________
>Brian Guralnick
>
>
>
>----- Original Message -----
>From: "Brad Velander" <[EMAIL PROTECTED]>
>To: "'Protel EDA Forum'" <[EMAIL PROTECTED]>
>Sent: Wednesday, June 13, 2001 5:50 PM
>Subject: Re: [PEDA] Microwave PCB layout
>
>
>| Brian,
>| more on our (my) methodology. Typically we import DXF or Gerber from
>| our RF design/simulation tools. I prefer DXF because Gerber typically has
>| too many individual drawn elements making up everything. I then use the DXF
>| as a template and duplicate the circuit using traces where applicable and
>| fills where square ends are required or the copper element is square or
>| rectangular.
>| Using the DXF I can usually pop the curved line portions to the
>| conductor layer and don't have to enter the curves through Protel. Then I
>| can attach a regular trace to the end of curve for a perfect match. The DXF
>| rectangles and squares typically come in as fills (unless they are rotated)
>| and again I pop them onto my conductor layer. The fills which are rotated
>| come in as outlines or a polygon type outline and I will carefully replace
>| these with rotated fills on my conductor layer, using the original as my
>| guide.
>|
>| Brad Velander,
>| Lead PCB Designer,
>| Norsat International Inc.,
>| #300 - 4401 Still Creek Dr.,
>| Burnaby, B.C., V5C 6G9.
>| Tel. (604) 292-9089 direct
>| Fax (604) 292-9010
>| website www.norsat.com
>|
>|
>| > -----Original Message-----
>| > From: Brian Guralnick [mailto:[EMAIL PROTECTED]]
>| > Sent: Wednesday, June 13, 2001 2:08 PM
>| > To: Protel EDA Forum
>| > Subject: Re: [PEDA] Microwave PCB layout
>| >
>| >
>| > The most annoying thing about this is that if you make a PCB
>| > with the rounded ends, make the gerbers, edit the circles to
>| > rectangles in the apertures in beginning of the Gerber file,
>| > import the Gerber file into a new PCB, you will have the
>| > square ends which you want.
>| >
>| > _____________
>| > Brian Guralnick
>| >
>|
>|
[EMAIL PROTECTED]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
