Protel : PWB design release to manufacturing (CAM)

prev: PWB_libraries.htm -- next: format_conversion.htm

design release to manufacturing (CAM)

You generally want to archive the "original", "as-released" version of the files just before you generate Gerbers. Here is one common sequence:

1. Exit Protel. From the "File Explorer", right-click-and-drag on the ".ddb" file (or on your design folder), drag slightly, and select "Copy Here" from the pop-up menu. This creates a "Copy of ..." file in case I go click-happy in step 2.
2. Double-click on the ".ddb" file, starting Protel. Click on the "Documents" tab. Delete the old "CAM for ..." folder and those obsolete ".txt", ".rep", "Copy of ..." files. Click on the "Recycle Bin" and empty it.
3. Click on the little down-arrow icon just to the left of Protel's "File" menu. Select "Design Utilities". When the "Compact & Repair" dialog box appears, activate "[Y] Perform Compact after closing design | Close".
4. Exit Protel. It churns for a long time "compacting". Some people find this so annoying that they usually disable "[ ] Perform Compact after closing design". Then (from the "File Explorer"), right-click on the ".ddb" file, select "Properties", and activate "[Y] Read-only | OK". You will note that this file is *much* smaller (1/4 the size is typical) than your previous "Copy of ..." file, even when it contains exactly the same files. Archive copy(ies) of this file somewhere safe (a write-once CD-ROM ?). (I think Protel 99SE s.p.6 was the first to be able to read read-only ".ddb" files)
5. Double-click on the ".ddb" file, starting Protel. If you have it already, click the ".cam" file and hit F9 to generate Gerbers. Otherwise, use Tools / Preferences to first set the output directory; Some people archive these in the same place as the ".ddb" from step 4. Then run the Cam wizard from the Tools menu to setup the desired outputs. There are many options which should be discussed with the board house in advance.

Just before sending these Gerbers out, it's a good idea to go through a check list http://www.baldwin-tech.com/Checklist.htm /* was http://www.baldwin-tech.com/designgu.htm */ . Most people have a text file associated with each project listing ``things to remember to do before sending out the Gerbers''. [FIXME: other useful check lists ?]

``Standard Operating Procedure for Protel users should be, before releasing a job for production, to reload the net list and see what macros are created. Normally, if *any* macros are created, it means that something is wrong.'' -- Abd ul-Rahman Lomax on 2001-01-30 03:42:55 PM

Some board houses want a ``SMD pad count'' to help them calculate their price quote. Under ``Reports | Board information... | Report...'' there's lots of data. Dennis Saputelli takes the number of pads+vias and subtracts the number of holes to get the ``SMD pad count''. Some people think that the ``pad paste mask'' ought to equal the ``SMD pad count'', since paste is only needed on SMD pads. But Protel apparently puts paste on every pad, even through-hole pads. (This is a feature if you're using pad-in-paste to solder your through-hole components).

http://www.schablone.de/ is one of the companies that makes Paste stencils.

Now you have all the files you need to send to your PWB manufacturer ../pcbfabs.htm , plus a stencil file to send to your assembly house.

While they are making the board and the stencil, check the BOM, order parts, print an archive copy of the schematic.

printing schematics

Besides printing to a printer, lots of people "print" to ".pdf" files. PDF

1. I use only A4 size schematics. That implies almost every time using a
hierachical design. Not everybody's taste, I know.
2. We use Adobe Acrobat documents (*.PDF) and email as our main way of
communication. That's a way most customers can deal with, and the resolution
should be good enough even with downsized A2 documents.

-- Heiko Vachek elektronik 21 GmbH on 2000-08-23 06:34:32 AM

If you have a choice, don't
draw A2 schematics or larger, they are more hassle for everyone. Few people
now have large enough format printers and copy machines. If the text size
is large enough, an A2 might be readable on a fax in fine mode if directly
sent (not printed to paper first).

-- Abd ul-Rahman Lomax on 2000-08-23 03:36:51 PM

What I do is to use Adboe Acrobat 4.0 for a cost of $250.00.  Using this allows me to
create a .PDF file in which anyone can read with an Acrobat reader which seems to be
the Internet Standard.

-- Dave Adams on 2000-08-23 07:02:08 AM

then the ONLY thing you need to do is "print" out your protel
schematic, but select the pdf printer, and instead of a hardcopy you
get the pdf files.  refreshingly simple in a world filled with complex
solutions.

-- Robison Michael R CNIN on 2000-08-23 06:59:45 AM

Ghostscript is a free postscript viewer with the ability to convert postscript files to PDF.

Not quite so convenient as Acrobat, but then it only costs a download.

Start here http://www.cs.wisc.edu/~ghost/doc/faq.htm and get Gsview also.

... with P99SE sch, pcb files printed to .prn files. After conversion with GSview from prn to pdf files, all is readable and "zoomable" with the free Acrobat Reader. Your solution work fine with "big" sheet format too. ... -- Rudolf Schaffer on 2000-08-24 05:19:06 AM

You can also make PostScript files, and view with GhostScript,
or print on any PostScript printer.  These will come out quite sharp,
even printing a B-size schematic on A paper.

-- Jon Elson on 2000-08-23 05:04:22 PM

• Q: When I generate a PDF file from a Protel Schematic, sometimes the overbars are misplaced. How do I get them to print correctly ?

  A1: ``I have found that I can avoid the relocated overbars by ensuring that PDFwriter is configured to embed all fonts, with no exclusions. It makes the PDF a bit bigger, but at least I have a distributable schematic!'' -- John Haddy

  A2:

  ``it appears that the "relocated overbars" go away when the sheet to be printed is OPEN before printing. Not a problem for single-sheet schematics. Messier for big hierarchies.

  I still agree that the overbar is a bad crutch and should be avoided, but if you're in my boat where cleaning up old designs (renaming pins and net names to remove the \ before each character) may cause more problems than it solves, this is not a bad fix.''

  -- Drew Lundsten

PDF

Many people export Protel schematics to .PDF files. Two methods: (a) "print to file" using a Postscript printer driver, then using (freeware) Ghostscript to convert to .PDF, or (b) using Adobe's proprietary software.

Q: Has anybody figured out a way to print a batch of PCB .PPC files so they end up as pages in a .PDF file? Works nicely when printing the pages of a schematic project. -- f12

A1: Run the PcbPrint:PrintDocument Process with the parameter of:

  Action=PrintAsSingleJob

This will produce one Acrobat file for *all* of the defined Printouts, rather than an Acrobat file *per* (defined) Printout.

In the default (Power Print Server) menu, select 'File/Print Job' to produce this outcome. -- Geoff Harland.

A2: I figured out that in 'Browse PCB Print' under the listed printer you go to Properties>Insert Printout, then you can set up other printouts which will be printed as separate PDF pages from the same .PPC file. -- f12

Q: How do I arrange the order of the sheets in a project so that they are in the order that I want, and that they print in that order ? -- lloyd A:

`` ... with the Edit/Move/Send to Back and Edit/Move/Send to Front commands.

The schematic pages print out in the order that they are displayed in the hierarchy display on the Explorer window. By selecting 'Send to Back' and clicking on a sheet symbol [the sheet symbols on your top-level block diagram schematic] , you actually push it to the top of the hierarchy and make it print first. I normally go through my schematic and start by clicking on the last page that I want to print out and click on them one at a time until I get to the first page. (You could start with the first page if you used the Send to Front command instead).

Note that to get the hierarchy window to update, you need to right click on the DDB and select refresh. ''

Gerber

Nearly all PWB designers generate Gerber files of their layout to send to the board house for manufacturing.

Q: "Is there any way to direct the Gerber outputs to a location of my own choosing?" -- Steve Allen

A: Click on the ".cam" file, so you see the things it's about to generate with the little square checkboxes. Then hit "Tools | Preferences...", and in the section titled "Export CAM Outputs", hit the button labeled "..." and select the appropriate location on your hard drive. If you haven't set up CAM yet, it's easy. While viewing your PWB in the editor, hit "File | CAM Manager". This starts a Wizard that asks a bunch of nosy questions, and when you're done there should be a new ".cam" file in the "Documents" folder. Once you're done, you'll probably want to right-click and select "Insert NC Drill"...

Q: While looking at the Gerber files (using Camtastic or another Gerber viewer), the drill points don't line up with the other layers !

A: While looking at the CAM file "CAM Outputs for...", right-click on "Gerber Output", select "Properties | Advanced", and disable "[] Center plots on film".

Q: What does activating "[X] Center plots on film" do ?

A1: It doesn't help anyone, and it only leads to confusion when you try to view these plots with a Gerber viewer. "Never, ever, turn on the "center plots on film" option when generating Gerbers." -- Steve Hendrix"

A2: "It gives an offset to the gerber data such that the plot will be centered on the film. Thus such a plot will not match the drill file, which has no offset." -- Abdulrahman Lomax

Gerber viewers

Board houses want to feed Gerber files into their plotter machines. It might be a good idea for you to look at the Gerber files that Protel creates before you send them to the board house.

Gerber file viewers (not in any particular order)

[FIXME: would like short review comparing these tools]

"Have a look at http://www.camcad.com/ for CAMCAD viewer for Protel, Accel, DXf, HPGL and more" -- Wolfgang [Apparently this views the Protel ".pcb" file format as well as Gerber, DXF, etc.]

GerbTool http://www.gerbtool.com/ [FIXME: offline ? http://core.bisc.com/demos/GerbToolSR5.exe ]

GraphiCode, Inc. : GC-Prevue 8.0 Win95/NT http://www.graphicode.com/

Lavenir Technology, Inc. : ViewMate http://www.lavenir.com/ | ftp://ftp.lavenir.com/Updates/ViewMate/ also has a "Gerber to PostScript Converter" ftp://ftp.lavenir.com/FromLavenir/lfilm.zip

http://www.sss-mag.com/cad.html http://www.sss-mag.com/zip/camcad.zip

Router Solutions, Inc http://rsi-inc.com/ | http://www.rsi-inc.com/camcad.html#FreeCAMCAD | ftp://ftp.rsi-inc.com/pub/demo/win/CCShare.exe | http://help.camcad.com/ | http://www.camcad.com/

Camtastic [now bundled with Protel]

These web sites have lists of Gerber file viewers: http://freeware.intrastar.net/graphics.htm http://www.cctc-pcb.com/cctc/download.asp

Reviews:

"the Camtastic stuff is pretty good. The
new 2000 LT (the full 2000 isn't out yet) works well for me.
...
Like it a lot more than the Lavenir stuff I've got. Most PAD's houses I know
use the old DOS Lavenir and swear by it. I guess it's a matter of choice.

As to bringing in the drill file into Camtastic, it allows you to select and
snap the move to the board reference (either outline endpoint or object
center if you use a ref hole)."
--
WAM
http://home1.gte.net/wamnet

part fields and the bill of materials (BOM)

See also part_type

Q: ``what's the best way of generating BOMs ?'' -- Matthew

A: ???

Many people export a BOM and manually pretty it up in Excel. We all wish there was an automated method.

If you export to ".csv" format, the ".csv" file has to be renamed to a ".txt" so that Excel can import it using the import wizard. Otherwise it will assume 'general' fields and make an 'E' an exponential and truncate size "0603" to "603". -- chris.mogford

Terry Harris http://www.harrt.btinternet.co.uk/electron.html is giving away an AWK script to re-format the Protel BOM .CSV files into whatever you like. "I set up a file association for .CSV files to run the processing batch file on them so a formatted part list is only a couple of clicks away." The description field can be any combination of part fields and text you like and the partlist is alpha sorted on the description. -- Terry.

IONOS http://www.ionos.com/ sells a parametric part database "dCSM" that supposedly interfaces with Protel to generate pretty BOM files -- an excel2000 file in the format you prefer. -- chris.mogford

In Protel99(SE) importing an excel spreadsheet into the ddb automatically truncates each field to 256 characters. ie. unless you have very small boards do not use the protel spreadsheet function. Worse than useless, it is dangerously wrong. The moral is: "Only use the csv renamed to a text BOM function. Nothing else" -- chris.mogford

For complete accuracy, we use the schematic as the reference. It includes the screws, heatsinks, heatsink compound, etc. We use Part Field 16 for a Company Part Number. This then references manufacturer number etc. A typical excel BOM after massaging would have these columns : Quantity|Designators|Company no.|Manuf.|distributor|footprint|part type|part field 1|part field2.

-- Chris Mogford

Part information: Some people put most of this information into the schematic fields of the part. Other people just stick a (internal) reference number in the schematic, then put all this information in a seperate database / excel spreadsheet / text file to look up by reference number. Yuri V.Potapoff http://www.rodnik.ru 2001-08-03 and "chris mackensen" 2001-08-03 mentioned some of this information:

• Group
• Name (it isn't Protel's Type!)
• Type (it is Protel's Type too!)
• Nominal value (it isn't Value!)
• Tolerance
• TU refererence (specification No)
• Embodiment (not just footprint!)
• Work Temperature
• Limiting temperature
• Price
• Manufacturer
• Vendor
• Notice
• IBIS model
• URL to datasheet PDF file
• Spice Model and extra parameters
• normal part / prototype-only part / hand solder, do not pick-and-place / Only on model A / Only on model B /
• etc.

More part field tips:

• Q: ``How do I hide part fields on my schematic ?'' --Steve

  A: To hide an unwanted field:

  1) right click on the offending field,
  2) check the Hide field,
  3) click OK.
  
  To show a part field that is not currently showing:
  1) right click on the part,
  2) check Hidden Fields,
  3) click OK,
  4) right click on the field-of-interest,
  5) uncheck Hide,
  6) click OK
  7) right  click on the part,
  8) uncheck Hidden Fields,
  9) click OK
  

  Richard B Mc Donald" on 2001-01-09
• ``the "Sheet Path" field should be blank (or *) unless you know exactly what you're doing with hierarchical design.'' -- Steve Hendrix

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

Questions:

• mehuli21 at -Remove-yahoo.co.uk asks: " can i get job if i have knowledge of gerbtool version 10" +

Comments:

• anna.m at -Remove-clear.net.nz

  http://www.pwrtrnx.com Converting gerber files output from other pcb layout packages to protel 2.8 files. Go to Pwrtrnx.com they offer a service - I tried it - it works..!

  +

  .