******************************************************* Todays forums are sponsored by Ian Martin Limited Engineering/Technical Placement Specialists www.ianmartin.com *******************************************************
> > I'm designing a PCB that has multiple ground planes. To make it > > easier to assemble and rework I made the thermo relief with only 2 > > entries. No problem Protel will let you set them in PCB editor > > RIGHT??? I'm now viewing the board house generated Gerber and guess what > > " All plane connections have 4 entries. When back to PCB editor and > > imported my protel generated gerbers and they all have 4 entries. Then > > checked my original design in the PCB editor, it still has only 2 entries. > > > > Have I done something wrong? > > If not, how do I generate gerbers to look like the PCB in the PCB editor? > > > > Mark Witherite > > No, you have done something right. You have identified another bug, I just > verified it. I have not explored the boundaries of this bug, but I set a > pad-scope rule for 2 thermals when the board-scope rule was 4 thermals. > Display of the ground plane was correct, the special pad showed 2 thermals > and all others showed 4. However, in the gerber, all connected pads had 4 > thermals. > > In other words, the gerber generation routine is broken here. A moderately > harmless bug unless you really need differing thermal connections on a > board, in which case it is downright irritating. > > (Once again, the rarity of this explains why we have been staring at this > program for a long time and had not yet found this bug.) > > Abdulrahman Lomax This situation can be regarded as a shortcoming of the RS274X standard, in that Aperture Macros of a Thermal (Relief) type provide no means of defining how many sections (entries) this type of pattern has. As such, one "correct" way to have a PCB manufactured with the appropriate number of entries (for all thermal relief shapes) is to create Gerber files *without* embedded aperture definitions (i.e. RS274D format rather than RX274X format). The PCB manufacturer will then need to be provided with not just the Gerber files, but *also* an aperture definition list file. (When the RS274D option is selected, an aperture definition file is generated for *each* Gerber file. However, all of those (aperture definition) files have the same contents, so it is only necessary to retain and send one of those (aperture definition) files, which should have its extension changed to .APT.) In Protel 98, it was possible to select whether Thermal Relief patterns were "flashed" or "drawn"; with the former option, apertures having Thermal Relief patterns are used; with the latter option, the arcs of each thermal relief pattern are "drawn" using an aperture of round shape. As such, *if* Protel 98 is being used, RS274X format Gerber files *can* be created, but the "Generate Relief Shapes" checkbox within the "Apertures" dialog box needs to be put in an *unchecked* state. (Note that because these patterns are now being "drawn" rather than "flashed", the Gerber files (for the Power Plane layers) will be larger than would otherwise be the case.) In Protel 99 SE, the "Apertures" tab of the "Gerber Setup" dialog box (invoked from the "CAM Manager" server) does incorporate a "Generate Relief Shapes" checkbox, but this checkbox is *only* enabled when the "Embedded apertures (RS274X)" checkbox (on the same tab and same dialog box) is *not* checked. If you are generating RS274D format (Gerber) files (no embedded aperture definitions (within the Gerber files)), it is not necessary to deselect the "Generate Relief Shapes" checkbox, as you would then need to provide the PCB manufacturer with an aperture definition file, and that would specify that some of the Thermal Relief apertures have just two entries rather than four. (Having said that, it could still be preferable to still deselect that Checkbox, as it would reduce the probability of the PCB manufacturer "stuffing up" your PCB by not using thermal relief patterns with the correct numbers of entries. The Gerber files (for the Power Plane layers) will be larger, but better that than receiving mis-manufactured PCBs.) However, the ability to create RS274X format Gerber files (with embedded aperture definitions) in which thermal relief patterns are "drawn" rather than "flashed" does seem to have been lost in Protel 99 SE (unless someone can verify that the state of the "Generate Relief Shapes" checkbox is acted upon even when this is disabled), and this is definitely a shortcoming in cases where the PCB designer wants thermal relief patterns that have just two entries (rather than four). Altium please note!!! If you know what you are doing, it is still possible to create Gerber files *with* embedded apertures; most PCB manufacturers will thank you if you do that (as that saves them from having to define the details from the contents of the aperture definition file). You could create a Perl script (or similar) which adds aperture definitions to the Gerber files (so converting them from RS274D format to RS274X format). And perhaps the "old fashioned" way of producing Gerber files (i.e. from invoking the Pcb:SetupPrinter process) is still sufficiently "unbroken" to permit you to generate RS274X format Gerber files with "drawn" thermal relief patterns. In cases like your PCB, which uses thermal relief patterns with just two entries, it would be highly desirable to produce Gerber files yourself, rather than sending the PCB file (instead) to the PCB manufacturer and having them produce Gerber files for the PCB. (And if you do send the PCB file to the PCB manufacturer, you should specifically point out that some of the thermal relief patterns have just two entries rather than four, so that they don't "stuff up" on that aspect.) And if you send RS274D format Gerber files, you should yet again point out that the (also provided) aperture definition file contains thermal relief patterns having just two entries rather than four. I have yet to design a PCB in which I have wanted thermal relief patterns having just two entries rather than four. Having said that, I always generate my own Gerber files, and then always preview these, using GC-Prevue, before sending these to a PCB manufacturer. (There are other previewing utilities available other than GC-Prevue, including the version of Camtastic provided by Altium, but I have long been accustomed to using GC-Prevue for this purpose, and it is *totally* independent of Altium (though for the time being, that aspect is essentially nominal in nature).) The moral of doing that is that you are far less likely to be "surprised" by what you receive back... Pads having an octagonal shape also need to be "handled with care". As such, I never use octagonal pads having differing widths and heights (once again, the RS274X standard does not handle the associated shapes in a straightforward manner), and when I do use octagonal pads having equal heights and widths, I always "tweak" the associated embedded aperture definitions (within the Gerber files) to make these comply with the RS274X standard. (I also tell the PCB manufacturer that the Gerber files have been "tweaked", and why; some PCB manufacturers are apparently accustomed to receiving Gerber files which have been created by Protel and which have *not* been subsequently "tweaked".) I can't recall the URL off-hand, but it is possible to download a Rs274xrevd_e.pdf file from the Internet which specifies assorted aspects of the RS274X standard. Familiarising yourself with this file's contents will alert you as to why alertness and care is required with thermal relief patterns and pads having an octagonal shape... Regards, Geoff Harland. ----------------------------- E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
