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 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 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 . 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 - 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 . - 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 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 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.