Yes, I would agree ths to be the best practice.
We leave the outline on only for internal purposes really.
Paul.
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Mark Koitmaa
Sent: lunedì 19 maggio 2008 21.09
To: [log in to unmask]
Subject: Re: [DC] FAB:CAD2CAM
I do not include the outline on each layer. I supply the outline in a separate layer file.
I began this practice after working as a CAM operator for awhile because the first thing we did was to remove the outline from all the layers and create a separate outline file.
Mark
On Sun, May 18, 2008 11:51 pm, Di Marcello Paul wrote:
> No problem Jack.
>
> I leave the outline on all layers like Mathew does.
>
> I do supply, together with the drilling, the profile with more
> detailed instructions for the routing.
> i.e. internal radii or critical dimensions with tolerances, hole to
> edge etc.
> Most times this has never really been a problem though. Just covering
> my ass.
>
> The last software I used was by Valor.....Genesis.
> This, like I think most modern CAM softwares has an easy to use,
> almost automatic rout file creator.
> The CAM guys basically use the outline provided off one of the layers
> to create this....then give it a check afterwards.
> Usually a very quick procedure.
> Not really for us to worry about much......
>
> Paul.
>
> ________________________________
>
> From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of
> Jack Olson
> Sent: venerdì 16 maggio 2008 17.59
> To: [log in to unmask]
> Subject: Re: [DC] FAB:CAD2CAM
>
>
> Thanks for taking the time to respond, I really appreciate it.
>
> I too have heard that there is more difficulty with drilling file than
> with Gerber files, and I usually don't even load that one into my
> viewer. I will definitely mention that...
>
> One question I meant to ask... do any of you create the file that cuts
> the board out of the panel, or do you let the supplier do it? What is
> that called anyway? Mentor calls it "MILLING" data, but I hear others
> refer to it as the PROFILE, but neither of these is in IPC-T-50. For
> the record, I found the definition of ROUTING in there and ROUTING
> MARKS, which might confuse people who use auto-routers all day.
> The CAM people I have talked to all say they discard mine even if it
> exists and createtheir own, but I don't want to make a blanket
> statement like that if not everyone is doing it that way.
>
> Does anyone use routing marks? (I haven't since the 80's) Do you leave
> the board outline in your Gerbers or not?
> Just on the mask layers maybe?
> To me, it seems sensible to have the outline line in the soldermask
> for reference.
> (maybe even a fatter line so the mask it "backed away"
> from the edge a few thousandths.)
>
> onward thru the fog,
> Jack
>
>
> .
>
> On 5/16/08, Di Marcello Paul <[log in to unmask]> wrote:
>
> I used to work also in the CAM area of various PCB manufacturers.
>
> The ODB++ thing surprises me also....they were talking of this years ago.
>
> The thing is....from my experience...extended gerber was sufficient
> for the CAM guy. It was a big improvement from the older non-extended gerber.
> Obviously the biggest problem with the older gerber was the aperture
> lists. Quite a lot of the times these had to be manually typed in and
> because of this, most times, 2 guys were needed.
> One to read, one to type, then double check....lots of room for error.
>
> There could be that there are still minor problems reading in the the
> drilling data.
> Again from my experience in the past, this data could come in all
> sorts of formats
> (Excellon...Sieb&Meyer....then...2,4...2,3...3,2....inch.....metric...
> leading zero or trailing zero suppression etc....).
> This required some kind of trial and error. And if all else
> failed....create this file from the pads off one of the layers.
>
> Regarding modifications...again from my experiences...
> Via hole diameters were always preferred that they could be left up
> to the manufacturers discretion so as to optimize the annular ring and
> therefore registration.....
> Often the finished diameter, detailed on the drill drawing, would be
> considered as the DRILL diameter.....therefore 0.10 to 0.15mm smaller
> for the FINISHED size.
>
> Small changes.....we are talking of pad small pad increases
> etc.....could be changed without notification....depended much with
> the client....some were more picky than others....
>
> Usually any type of track movement or major errors were reported back
> to the designer so that he/she could modify the source files.
>
> Most times the apertures for the solder resist layers were "Blown"
> without notification.
> If asked it was always stipulated that the solder resist apertures be
> one to one with their respective pads so then after the aperture
> increases they would be uniform in size throughout the board.
>
> Regarding silkscreen...
> If the board was going into quite high volumes then there was the
> need to shift the identifications of the components slightly so that
> they wouldn't get clipped....and therefore be illegible.
>
> Small volume prototypes...most times....no modifications....and it
> was just clipped.
>
> Etch compensation was always applied.
>
> If there was a modification that notification was needed....usually
> then....all modifications were reported....even the slight ones....but
> generally....not too much detail.
>
> Anything critical....the production was put on hold until further
> notice from the designer.
>
> It has been quite a few years since I was in this field.....some
> things and approaches have most probably changed.....and also these
> approaches could change from manufacturer to manufacturer.
>
> Now I'm a PCB designer this experience has helped me greatly in some
> aspects of my designs. And so far, fingers crossed, no questions have
> been asked.
>
> The opportunity presented to you Jack, I would recommend very much.
>
> Just one day sat with an experienced CAM guy is very helpful.
>
> Paul Di Marcello
> PCB Design Engineer
>
> Pepperl+Fuchs Elcon srl
> Via delle Arti e Mestieri, 4
> 20050 Sulbiate (MI) ITALIA
>
>
> ________________________________
>
> From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of
> Jack Olson
> Sent: mercoledì 14 maggio 2008 22.29
> To: [log in to unmask]
> Subject: [DC] FAB:CAD2CAM
>
>
>
> I've recently had the opportunity to spend some time with "the CAM guy"
> at our primary circuit board supplier, and now a magazine has
> expressed an interest in publishing an article about what happens to
> data as it moves from CAD through CAM. If any of you are involved in
> this process, here is a golden opportunity to voice your concerns (or
> your "wish list"). I already have my notes for what happens to OUR
> data, but I would like to be more generic for the magazine.
>
> If you aren't doing CAM work but know someone who might like a shot
> at this, PLEASE forward this to them.
>
> The most surprising thing I learned this week was the extremely low
> percentage of jobs being submitted in an intelligant format. For
> example, we've been told for years to move to something like ODB++ or
> GENCAM, but I'm hearing that maybe only a few percent of the jobs are
> anything other than regular old Gerber. Is that true? Would it help
> you significantly to get some alternative to Gerber?
>
> I'm also interested to hear anyone's thoughts on the note that can be
> found on many drawings that says:
> "DATA SHALL NOT BE MODIFIED WITHOUT WRITTEN APPROVAL".
> Where do we draw the line on that?
> Plot film with data "AS IS"?
> How does it apply to
> etch compensation?
> removal of non-functional pads?
> teardropping?
> silkscreen clipping?
> What is "standard" editing, and what really should be pre-approved?
>
> We've been told to always place the origin on a tooling hole. Does it
> really matter?
> Would you rather have the soldermask 1:1 with the pad size and
> enlarge it yourself?
> Would it help you much to have positive planes drawn with unique
> aperture sizes?
> Does the format matter? inches? metric? consistent with drill?
> Would it help to have better README files that explain more of our
> intentions?
> (like a known netlist discrepancy, for example)
>
> What do you wish more people would do to make your life easier?
>
> Maybe its inconvenient to answer so many questions, but if we have a
> chance to teach designers what we want, shouldn't we try?
> (I'm gonna write it with you or without you, so don't complain if
> what gets published is off-grid)
> Also, If I didn't ask the question you want to answer, don't hesitate
> to add to the list!
>
> If YOU were King of the World for a day, what would you change?
>
> Thanks in advance,
> I'll try my best to write a fair and thorough article
>
> Jack
> [log in to unmask]
>
> ----------------------------------------------------------------------
> --------- DesignerCouncil Mail List provided as a service by IPC using
> LISTSERV 1.8e To unsubscribe, send a message to [log in to unmask] with
> following text in the BODY (NOT the subject field):
> SIGNOFF DesignerCouncil
> To temporarily stop/(start) delivery of DesignerCouncil for vacation
> breaks send: SET DesignerCouncil NOMAIL/(MAIL) Search previous
> postings at: http://listserv.ipc.org/archives Please visit IPC web
> site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
> for additional information, or contact Keach Sasamori at
> [log in to unmask] or 847-615-7100 ext. 2815
> ----------------------------------------------------------------------
> ---------
>
>
> ----------------------------------------------------------------------
> ----------- DesignerCouncil Mail List provided as a free service by
> IPC using LISTSERV 1.8d To unsubscribe, send a message to
> [log in to unmask] with following text in the BODY (NOT the subject
> field): SIGNOFF DesignerCouncil.
> To temporarily stop/(restart) delivery of DesignerCouncil send: SET
> DesignerCouncil NOMAIL/(MAIL) Search previous postings at: www.ipc.org
> > On-Line Resources & Databases > E-mail Archives Please visit IPC web
> site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
> for additional information, or contact Keach Sasamori at
> [log in to unmask] or 847-615-7100 ext.2815
> ----------------------------------------------------------------------
> -----------
>
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d To unsubscribe, send a message to [log in to unmask] with following text in the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL) Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
