Pg1

A Cook Book for GCPrevu

This document is not intended to replace the information provided
with the software.  It's intent is to simplify first time operations.  
The viewer can display both gerbers and nc drill files in a composite mode. 
This will allow you to inspect all aspects of your fabrication data.

Requirements - PC/DOS based system with vr 4.xx or higher, hard drive with
               about 10 meg free space for both the program and work files,
               VGA monitor or better, mouse or other pointing device.
               A good ASCII data viewer.

Data -         GraphiCode's product can read both RS-274D and RS-274X 
               gerber data as well as NC drill files in Text (ASCII)
               and EIA formats.  There are others that the documentation
               provides details on.  The focus of this collection will
               cover RS274D and X versions and drill data in ASCII text.

Suggestion -   Place all program files and aperture conversion routines
               in the same directory.  Add this directory to your DOS Path.
               Create a small, simple named, batch file to activate the program
               for example GCP.BAT.  The batch file should contain the drive and
               path eg."c:\pred1\gcprevue", this allows you to activate the
               program from any directory on your drive(s).  Also you should
               acquire a copy of the aperture conversion utilities and place
               them in the directory as well.  This will eliminate many hours
               of aperture typing in the long run.  Not to mention reduction
               of key-stroke errors.

Apertures and stuff.

          GCP, (short for GCPrevue), will only load apertures formatted
          by one of the conversion utilities.  IT WILL NOT LOAD aperture files
          generated by your cad system directly, they must first be converted
          by using one of the external utilities in the GCAPTCNV.ZIP file
          available from AP Circuits BBS or INET HomePage. (You could
          get it from GraphiCode too I suppose).  If your cad system is not
          listed in one of the utilities, there is a user definable setup
          you can play with...or call GraphiCode's BBS (206) 771-6980
          Voice (206) 672-1980.  There may be a new release for your system 
          there, if not... happy typing.

          -OR- You may have a cad system that is capable of producing RS-274X
          data.  In which case the above won't apply.  RS-274X data contains
          a specific format header that defines all of the apertures and shapes
          during the loading of the data.  Much easier, kinda like post-script
          only different.  The following examples should help...

RS274-D (needs an aperture file converted or manually typed in)

D10*X13575Y5625D03*Y5825D03*Y6050D03*X13075Y5625D03*Y5825D03*Y6050D03*
D11*X10975Y7900D02*X10875Y8300D01*X11175Y7800D02*X11375Y7900D01*

End of Example
Pg2 Apertures and stuff con't.

RS274-X (automatic aperture file creation during loading stage)

*%FSLAX23Y23*%
%MOIN*%
%ADD14C,0.052*%
%ADD17C,0.125*%
%ADD800C,0.003*%
%ADD801C,0.007*%
%ADD802C,0.01*%
%ADD803C,0.05*%
%ADD804C,0.1*%
%LPD*%
D800*X11700Y400D2*X11900D1*X11700Y300D2*X11900D1*X400Y11700D2*Y11900D1*
X300Y11700D2*Y11900D1*X11700Y700D2*X11900D1*X11700Y600D2*X11900D1*X11700Y500D2*

End of example

OK that's out'a the way...next is the drill stuff...(don't worry..I'll get back
to the rest of gerber and apertures when it's time to start typing about loading
the data.)

NC Drill file stuff

Rule number 1 

- if you can't see your drill data in normal ASCII text with your "viewer",
...chances are pretty good that the software won't either.  There are few
exceptions to the rule.  Here is a sample of a normal ordinary drill file.

The following segment is from a Tango NC drill file header:

M48                 - Program Header - is ignored up to first "%"
INCH,LZ             - English measurement and Leading 0's
T03F00S00C0.038     - T03 is defined as .0380" diameter, no speed RPM or Z
T04F00S00C0.125     - T04 is defined as .1250" diameter, no speed RPM or Z
T06F00S00C0.046     - T06 is defined as .0460" diameter, no speed RPM or Z
T12F00S00C0.063     - T12 is defined as .0630" diameter, no speed RPM or Z
T16F00S00C0.250     - T16 is defined as .2500" diameter, no speed RPM or Z
%                   - Rewind and Stop (start of drill data)
T03                 - Drill COMMAND - GET TOOL 3
X+00581Y+0122       - Drill Plunge with TOOL 3
T06                 - Drill COMMAND - GET TOOL 6
X+01657Y+03295      - Drill Plunge with TOOL 6
T12                 - Drill COMMAND - GET TOOL 12
X+00585Y+03311      - Drill Plunge with TOOL 12
T04                 - Drill COMMAND - GET TOOL 4
X+00873Y+02691      - Drill Plunge with TOOL 4
T16                 - Drill COMMAND - GET TOOL 16
X+00625Y+02191      - Drill Plunge with TOOL 16
T00                 - Drill COMMAND - UNLOAD TOOL
M30                 - End of Program

If your NC output doesn't come close to the example above, then examine your
setup options and adjust as necessary.  The comments to the right will not be in
your data.  There may or not, be + or - symbols in the data, it's nothing to be
alarmed about if they are absent.  Also your NC system may not define the tool
diameters in the header - again not a problem, the primary information starts at
the % and ends at M30.  If your drill file contains a bunch of odd looking
graphic characters it's likely EIA format - you can load it as well...but it's
worth the effort to track down the ASCII flavour of the drill data...not all
vendors have every conversion utility available.Pg3

The Basics

     Please excuse the presumption that you are learning GCP for the first time.
The focus here is to get your program operating ASAP as well as giving you a few
"tricks" along the way.  This session is mostly a Key-by-Key review with out a
lot of details as to why the operation is necessary.  More to the point, it's
from the stand point of "I have gerbers and drill files...how the heck do I load
and view this stuff, with our sifting through 60 pages of doc files!".

Begin: start the program from the directory containing the gerber and drill
files.  (presumably you followed the suggestions on Pg1 labelled "Suggestions")

Layer Sorting Order

*.NCD layer 1, *.GTL layer 2, *.GBL layer 3, *.GTO layer 4, *.GBO layer 5, 
*.GTS layer 6, and *.GBS layer 7.  This sequence is optional, BUT recommended, 
as GCP hides smaller pads under bigger pads, so if the drill is loaded last
(smallest pads) you will not be able to see the annulus of the pad that is
covering it.  If you load the Smallest Pads First they will stack up nicely
and you will also be able to see the soldermask annulus around the foil layer
pads.  By-the-way, if you are ordering prototypes (currently no masking
options are available) then you would drop layers 4 through 7, or if you
are ordering non-prototypes that don't use all of the masks outlined, just
adjust the layer count as necessary and only load the necessary layers for
fabrication.

Setting Up for the Loading of Data

     - using the arrow keys (directional keys) or the mouse, select "Layers"
from the tool bar.  Your cursor is now on the right side of the screen under the
"Filename" heading.  Pressing F10 will provide you a Directory Mask, you may
replace the default of *.gbr with *.* to display the entire contents of the
directory.  Using the space bar will tag the files you wish to load IN THE ORDER
THAT YOU TAG WITH THE SPACE BAR.  Pressing <CR> after all necessary files have
been tagged will deposit the file names into the layers list.  

DO NOT LOAD THEM YET!  

First a discussion of apertures, GCP is really finicky about the chicken and the
egg... in other words, you may get everything ready to load BUT the aperture
file load is FIRST before data!

Aperture Loading

     - notice the heading labelled "Aps", it has a default letter of "A" under
it's heading.  This letter represents the APERTURE file in use on the particular
layer adjacent to it.  You could have up to 99 data layers loaded using a
maximum of 10 distinctly different aperture files.  A blessing for users of
Orcad and Pads-PCB.  Both of those programs will generate unique apertures for 
each data layer...unless you are skilled in the output operation of those
programs and already know how to create a common aperture file for all data
layers.  OK to the point, now that you have file names set into the layers list
we need to set the aperture letter that corresponds to each layer.

The following examples are going to use the premise of *.GTL for top layer,
*.GBL for bottom layer, *.GTO for top overlay (component id's), *.GBO for bottom
overlay, *.GTS for top solder mask, *.GBS for bottom solder mask, and *.NCD for
the ASCII drill file.Pg4

Aperture Loading con't.

Press the <esc> key to get the cursor back to the Tool Bar and select 
"Apertures" from it.  This area operates the same way the layers list does,
move the cursor to table A, pressing F10 opens the directory with the mask
default set to *.APR (APR is GCP's default file extension for GCP's native
aperture files). Use the space bar to select the desired file and press <CR>.
You should now have a file name loaded into Table A's slot.  Pressing F1 will
load the Aperture file.  If the ERROR MESSAGE contains "*.APR" is not a valid
apr file, then one of two things occurred, the wrong file was selected, or the
selected file is not yet converted into GCP's native format.  If all went well
and no error messages displayed, press F2 to open the aperture list.  You will
now see a list of apertures from D10 through to the maximum D999.  Your table
will not necessarily contain that many apertures, more likely, D10 to about
D150.

The other information in the list is internal to GCP's shaping and usage of the
aperture.  Moving the cursor over to the TYPE (use the TAB KEY) is used to
define the shape of the aperture (space bar will scroll through the list of
shapes, or one of the FUNCTION KEYS in combination with the SHIFT or ALT key
depressed to speed select the necessary shape - there is a table on the lower
1/3 of the screen detailing this).  Your shape should already be described
if a pre-converted table was loaded - or if not, this is how you manually enter
in the necessary info to hand-build the table.  Tab to the Dimensions section
and inspect the size of the aperture.  A number of .0499" is a default size
and if several of these same sizes are detected in this column, you would be
wise to get a hard copy of your aperture file printed and scroll through each
Dcode to ensure it's shape and Dimensions are correct.  Also, if the shape is
symmetrical like a Round, Square, Octagon, Draw, Slit, or Target there will only
be one set of Dimensions displayed.  If, on the other hand, an asymmetrical
shape is listed - Rectangle, Oblong, Annulus, Thermal, Custom, Custom Thermal
then a second column will be presented to provide the "Y" axis of the shape.  In
the case of a Custom Thermal you will need to define AirGap of the slits, the
inside dia. of the pad and the annulus..etc..etc.. another table appears on the
lower 1/3 of the screen detailing the required information necessary to create
the thermal.  I got a bit windy there just to keep from re-stating similar areas
of this topic in the event you don't have a conversion for your aperture file
and you need to enter things by hand...If this is your situation, load the
layers 1st. This way you need only define the used apertures instead of a table
defining all possibilities, press ALT+U to remove unused codes after data is
loaded (again only if you are hand building the table) then define what's left.

Aperture Loading for a COMMON APERTURE LIST con't.

Layer 1 - *.NCD - set "Aps" to the letter T to indicate Tool List (drills only)
Layer 2 - *.GTL - set "Aps" to the letter A to indicate Aperture list A
Layer 3 - *.GBL - set "Aps" to the letter A to indicate Aperture list A
Layer 4 - *.GTO - set "Aps" to the letter A to indicate Aperture list A
Layer 5 - *.GBO - set "Aps" to the letter A to indicate Aperture list A
Layer 6 - *.GTS - set "Aps" to the letter A to indicate Aperture list A
Layer 7 - *.GBS - set "Aps" to the letter A to indicate Aperture list A

Aperture Loading for a NON-COMMON APERTURE LIST

Layer 1 - *.NCD - set "Aps" to the letter T to indicate Tool List (drills only)
Layer 2 - *.GTL - set "Aps" to the letter A to indicate Aperture list A
Layer 3 - *.GBL - set "Aps" to the letter B to indicate Aperture list B
Layer 4 - *.GTO - set "Aps" to the letter C to indicate Aperture list C
Layer 5 - *.GBO - set "Aps" to the letter D to indicate Aperture list D
Layer 6 - *.GTS - set "Aps" to the letter E to indicate Aperture list E
Layer 7 - *.GBS - set "Aps" to the letter F to indicate Aperture list FPg 5 - Enough already let's get to it!

     - OK your aperture file is loaded (or in the case of hand built - created)
     - Select layers from the Tool Bar & press <CR>
     - Move your cursor to the Aps section, set the T list for the Drill Layer
       and set the rest of the Aps to match the necessary Aperture file(s)
     - Move your cursor to the Drill Layer (Not a gerber Drill - the NC version)
     - Press F1 & select Drill 
     - A new menu appears, the 3rd. line down is "Plotter:", using your     
       directional key move to the plotter field, if the field is blank
       or does not contain NCDRILL.PDF you need to change it.  Using the
       F10 key, open a directory mask of *.PDF, if you can't find any PDF files
       type in the full path back to the GCP directory, ie. C:\GCP\*.PDF, now
       press enter, you should see several "flavours" of PDF files.  Using the
       arrow key, scroll down the list, select the NCDRILL.PDF then <CR>.
     - Using the arrow key, proceed further down the list until you locate
       "Whole Digits" - this determines how many places Left of the decimal
       the program is to interpret, the next one down is "Precision", and
       it determines how many places Right of the decimal to read.   Next line
       is "Abs/Inc." it's normally left set to ABSOLUTE. 
     - Lastly the "Zero Suppress", using the SPACE BAR will toggle the different
       selections.  For Example 2.4 this data would look like; 021500 (2.15")
       and you would use the Zero Suppress set to "Trailing" as the ZEROS at the
       end of the 021500 could be ignored.  At this point, load the drill only
       and do a test view (F2), if all of the pads a squished into a small area
       of the screen, you are going to have to go back, unload the drill file
       (Crtl-M) then re-load it and experiment with the Whole digits, Precision
       and zero suppress, until it looks right - data runs the gauntlet from 2.3
       to 5.5 .  Typical Protel data is 2.4 Trailing, Orcad is the same, Tango
       is 4.4 Trailing, Eagle is typically 3.3 Leading...keep hacking it...it
       will eventually look right, and as an added bonus, each time you modify   
       the NCDRILL.PDF you can save the changes, over writing the original PDF,
       so later on, you will have the PDF set to your Cad system's      
       specifications - no more fiddling around with it.
     - OK so the drill's loaded, now the gerbers, which is pretty much the
       same routine, Press F1 to load, select Gerber, replace the word "ALL"
       on the next menu (Layers:) with the layer numbers you want to load;
       Assuming Layer 1 is the Drill, then 2,3 is the gerber data
       (the 2,3 is valid loading info - the system would load layers 2 and 3)
       Set the Plotter Type to GERBER.PDF (just like the drill above) and for
       The most part using 2.3 whole/precision should be ok. then <CR> to 
       load layers. F2 to view the data...you should have some resemblance
       of what you drafted on the screen.  If it looks good press <esc> to get
       back to the main loading screen, the press F6 to save all work in
       progress - Be sure the aperture table is completed and the Drill tool          
       file has also been defined (tool bar, select drills, select edit)
       If your data appeared un-registered on the F1 display, you can locate the
       offset error by going back to View and locate an easily identifiable pad. 
       Press CRTL+N to snap to the centre of the pad, press "Z" to zero user co-
       ordinates, locate the mate to the pad you snapped on the next layer,
       press CTRL+N, observe the co-ordinates provided, feed those back into the
       X/Y offset table on the main loading screen.

       That's it...from here if you want more detail, consult the 60 page stuff.




































































