prev: PWB_release.htm -- next: protel_customize.htm#customize
(This page talks about converting files representing a PWB from one format to another file format. To convert that file to an actual physical PWB, see /techref/pcbfabs.htm )
There are tons of different CAD applications out there. ( ../pcbcads.htm ) If only it were easy to take information from one to the next, we could use each application for what it's best at. Why does each application need to have it's own slightly different email section ?
I'm listing the PWB CAD formats I'm most familiar with here. Feel free to add conversion tips for mechanical CAD and other CAD file formats. (Is there a file on massmind.org about converting between other file formats -- enhanced text, music, etc ?)
scottz at clearviewcatv.net asks: " How to convert dwg files to pdf format?
What software do I need and what are the steps?"
... Regards, Geoff Harland. ...
If you are switching from some other tool to Protel or back again, it would be nice if you could get all your schematics and PWB layouts into Protel and out again.
Protel to Orcad, Orcad to Protel, etc.
Converting your schematic into various file formats.
Converting your PWB layout into various file formats. [FIXME: should converting to ".pdf" files go here ?]
Q: [Can] Protel ... import gerber files from another design and turn it into a protel pcb? -- Brad Marshall
A: Camtastic http://www.camtastic.com/en/ (now bundled with Protel) can view most any Gerber file then translate it into the particular Gerber format Protel PCB editor can read. See
Importing Gerbers into Protel http://www.protel.com/kb/kb_item.asp?ID=2215 http://www.protel.com/kb/kb_item.asp?ID=1951 (was http://www.protel.com/kb/rdc2215.htm http://www.protel.com/kb/rdc1951.htm )
Q: I have a client who has a very old board ... [no gerber files] but he does have unpopulated pcb's. Does anyone know an easy way to generate Gerber files possibly with a scanner or something? -- Gary Allbee 2000-11-27
A1: Try Artnet http://www.artnet-tech.com/scan.htm . I have used them to scan films to make gerber files, then turned the gerbers into a circuit board. It worked well. They say they can scan actual PCBs. -- Vince Vlach 2000-11-28
A2: After scanning in the board, try this:
I photographed the board with a digital camera, processed the image to increase contrast and to scale it properly, and then imported the graphics file onto a mech layer in Protel using ...[ the BMP to Protel converter http://www.egroups.com/files/protel-users/Convert.zip produces polygons for the shaded areas of the BMP. ] ...
[Using that as a template,] I then placed parts and drew track to reconstruct the PCB. A net list was generated from the PCB and marked off against the schematic to find the few errors that were made in interpreting the image. In several places the actual PCB did not match the schematic, even though the board worked. That was not uncommon in the old days....
It is less expensive than doing a new design, but not a *whole* lot less.
-- Abd ul-Rahman Lomax 2000-11-27 07
I did it once this way. I had a only the film of a pcb and I had to do some modifications. ... scan ... Then I converted the bitmap with PCBLogo to a pcb-file. This looked already quite fine, but it wasn't exactly on scale. So I moved all the fills (PCBLogo converts to fills) to a mech-layer and draw the pcb on the copper layer and did the modifications. This PCB is now in mass production.
-- Edi Im Hof 2000-11-28 http://www.ihe.ch
Often component manufacturers have a ``reference design'' in Adobe's ".pdf" format.
Yuri V.Potapoff on 2001-07-31 08:46:06 AM wrote:
Step 1st is to convert PDF file to BMP by Photoshop. Then you can use Klipper utility from Desktop EDA (www.desctop-eda.com.au). This utility imports raster graphic file into PCB or SCH how array of fills (or lines). You need only adjust the scale. So you can get Gerber from Adobe' PDF file. We use this method to restore very old project or to copy another's boards. Then you can place footprints and generate netlist from connected copper. If you will have netlist you can add new layers and route pcb with your set of Desig Rules. You can see an example on our site. http://www.rodnik.ru/images/f_1_23_40b.jpg Best regards, Yuri V.Potapoff ... http://www.rodnik.ru
from Protel you first save the file in Orcad Schematic format)... =============================== From: Andrew W. Riley III Sent: Friday, January 05, 2001 5:28 PM To: Multiple recipients of list proteledausers Subject: Re: [PROTEL EDA USERS]: Protel to Orcad Schematic conversion Mr. Gulley, I am not sure about Express, but if you are attempting to import the schematic into Capture; The '.SCH' extension for OrCAD's schematic is for the older SDT version of OrCAD (IV & 386+). When opening '*.sch' files OrCAD expects to see the config file "SDT.cfg" in either the same directory as the schematic or the directories set by environment variables such as 'ORCADPROJ' in the autoexec.bat - created by the installation of OrCAD SDT. Though you should have one somewhere in your OrCAD (or sub-)directory, I have included the "SDT.cfg" that comes with OrCAD 9.2 at the end of this e-mail - just in case. I believe that Capture wants the libraries containing the parts used in the schematic. With version 9.x of Capture, it is possible to bypass the "SDT.cfg" file IF the SDT libraries are in the same directory as the SDT schematic. I have had to re-create symbols when I did not have the correct libraries, but the rest of the schematic(s) made it through. If I can be of any more help, please e-mail me at <drewmeister3 at earthlink.net> or ICQ me at 100686794 so as not to clutter Protel's list with OrCAD stuff.
"Abd ul-Rahman Lomax" on 2001-06-18 03:15:52 PM wrote:
Subject: Re: [PEDA] Importing Ocad At 02:07 PM 6/18/01 -0400, Steve Smith wrote: >Go to page 167 of the Protel 99SE manual and follow >the instructions there. They always worked for me. Another already mentioned p. 167 of the 99SE manual (which is available as PDF on the Protel web site). However, those instructions relate to Capture v. 9 imports. Other versions are more complex to deal with. My advice: using eCapture (see recent posts) import OrCAD -- any version -- to eCapture and write as version 9. Then import to Protel. Versions earlier than Capture require the presence of libraries and SDT.CFG. If you don't have the libraries, for these earllier schematics, you have almost no hope of import. Some of the data simply is not there. Abdulrahman Lomax
Protel will load Orcad Capture version 9 DSN files. If you look at a OrCAD file with a text editor, you usually can see the version near the beginning.
If you have some earlier version of Orcad DSN file, use eCapture 9.2 from http://www.spincircuit.com/download.html to load it in and write it out to version 9.
(see also microwave circuit layout tips #microwave )
import a DXF into an open PCB file. If you import the DXF into the database and try to open it then it does just stuff Protel. The DXF/DWG import into PCB is still not the most reliable of creatures even so. ... Usual Protel DXF import rules apply: everything MUST be in the positive quadrant and all must fit within the 100"x100" limits of the PCB.
-- Rob Malos on 2001-01-31 02:27:53 PM ....
Watch for the "scale bug". Sometimes Protel makes a file 24.5 times too big (or small ?). This seems to be a bug in the Imperial-->Metric conversion.
Sometimes when Protel doesn't want to import a DXF file, you can open it in Camtastic, then do "Open | Save" to create a ``new'' DXF file that Protel will accept. [tip from Darren Moore]
It's very easy to export Protel schematics and PWB layouts to Autocad DXF or DWG format. Then people can use freeware DXF / DWG viewers #dxf_viewers to view it, zoom in and out, etc., as well as importing it into most mechanical design packages to make sure the connectors, etc. on your board line up with the mechanical case.
While looking at the PWB layout, choose ``File | Export'', navigate to where you want the DXF file, type in an appropriate filename, hit ``Save'', then you'll get a dialog box. Choose DXF (or DWG) and you can change a few other options. Then hit ``OK'' and it's saved.
DAV: I prefer to export to ".dxf" format rather than ".dwg", because the exact same file in ".dxf.zip" format is smaller than in ".dwg.zip" format.
A1: I make my assembly drawings in Protel, then export directly to PDF. -- several people
A2: ``Before exporting from Protel make a scratch copy of the board, and then perform global edits on Tracks, Text, Designators, and Arcs that change the line width to 0. This greatly reduces the file size and redraw time. You also may want to change the linewidth of all Multilayer holes to 0 width in Autocad to get them to look a bit better.'' -- Andy Lintz on 2001-04-02
before exporting to any DXF/DWG I make everything 0 mil.This has another *major* benefit that the CAD snap points work correctly. A 10 mil wide track in Protel is made as a polygon in DXF/DWg which is no good for snapping to. You do need to make sure that the centre of you mech layer tracks is your PCB edge etc.
Also, I seem to recall that pads and holes etc are rendered in a very inefficient method - shown as filled (I do not know a better way of doing a filled circle in DXF/DWG mind you). To fix, once imported in my CAD package, I delete almost all the pads and vias - this makes a big difference. I will often place an arc on a mech layer around critical holes in the PCB - to shown the holes size and location and then make sure "export pads and via holes" is not checked - this helps keep the file size down.
I would like the option to export everything in draft mode to prevent this blow-up in file size and slow down in redraw. Everything would be exported as 0 thickness and pads/vias etc would not be filled (just arcs showing the copper annulus and hole size).
.... ....
I hate having to do global search and replace to set everything to 0 thickness - that is why I would like an "Everything-Exported-as-Zero-Thickness" ACAD export option.
Dimensioning errors due to snapping to vertices of polylines simulating non-zero line thickness may be small but are a source of confusion and sometimes can cause critical placement problems (step and repeat errors on panels might be one example).
A zero mil wide Protel track exports to ACAD with no-endcap and correct vertex snap points - this has made my dimensioning and export-to-industrial-designers life much easier and more accurate. As well as making my mech CAD program fly.
-- Ian Wilson on 2001-04-02 05:32:45 PM Ian Wilson on 2001-04-02 07:53:33 PM
"Steve Fallon" on 2001-08-02 10:33:12 PM wrote:
To: "Protel EDA Forum" Subject: Re: [PEDA] HELP. Converting old pcb I recently wrote a converter to take old CadSTAR boards and convert them in to ASCII Protel PCB 2.8. It works fine. It did need the CadSTAR board to be in its ASCII .cdi format, but I guess I could write one for the default binary .cdo. Let me know if you want a copy. Rgds Steve F
To: "Protel EDA Forum" Subject: Re: [PEDA] [PrU] Protel 99 PCB file format?
... a file format description, and I've uploaded it to the filespace for this list (which is a members-only space).
http://groups.yahoo.com/group/protel-users/files/Protel99SE_PCB_ASCII_File_Format.pdf
It's copyrighted by Protel ...
abd@lomaxdesign.com Abdulrahman Lomax
A:
1)Create a new DDB. 2)Add a new PCB 3) "File | Import | PADs Ascii (*.ASC)"
-- Mark Geddes 2000-11-27
end http://massmind.org/techref/app/format_conversion.htm
Interested:
Questions:
Comments:
See also: