For V-grooved, I use 1mm. Be careful when mixing V-grooved & different sized PCBs. You want to make sure that there is always a full length of panel material where you can break apart the PCBs with relative ease. Otherwise, the dificulty in trying to break off a PCB closed in on 2 sides may result in damaging a few of the PCBs due to stress when bending.
______________________ Brian Guralnick Vergent Technologies Inc. [EMAIL PROTECTED] ----- Original Message ----- From: "Yves" <[EMAIL PROTECTED]> To: "'Brian Guralnick'" <[EMAIL PROTECTED]>; "'Protel EDA Discussion List'" <[email protected]> Sent: Tuesday, October 17, 2006 11:35 AM Subject: Re: [PEDA] Generating panel of PCBs in P99se is super slow... > Brian, > > When you do your panel layout, what is the space you put in between board > when they are v-grooved. > > Thanks for the panel it looks quite good. > > > Yves Dubois > > Raytron LTD. > Montreal que. > > > -----Original Message----- > From: [EMAIL PROTECTED] > [mailto:[EMAIL PROTECTED] Behalf Of Brian Guralnick > Sent: October 17, 2006 9:59 AM > To: Protel EDA Discussion List > Subject: Re: [PEDA] Generating panel of PCBs in P99se is super slow... > > > The idea in preparing your own panel is to save set-up fees for each > 'different' PCB you are submiting. If you are sending replicas of just 1 > PCB, just tell your PCB manufacturer how you want it panneled & there is > not > price difference. > > Now, if you have something like 5 different PCBs, espicially when doing > prototypes, starting your own panel willcut your setup fees from 5 down to > 1. Your PCB manufacturer has no problems cutting them up. > > How To: > In step #1, I have a template, or, a set of margins drawn out on > mechanicle layer #1. These 2 sets of measurements you actually get from > your PCB manufacturer, 1 being the outer panel size & the border indent > where it is safe to start placing PCBs. Remember, to open all additional > layers you may need for the PCBs you may be using. I have not yet done a > panel with true power planes, in that case, you PCBs will need to have the > same net names. Remember to import design rules to get all your > paste/soldier mask/power plane expansions/clearances... > > Example: http://www.bigupload.com/d=89F6ABBE > > On all my PCBs, I place a border around them on mechanicle layer 1 > which > in my PCB description, I explain that the PCBs actual size relates to > those > borders. I use mechanicle layer 2 to place a larger box outsize of each > PCB > and 1/2 the closest safe distance between PCBs allowed. Get this > measurement from your PCB manufacturer. When copying & pasting, working > with electrical grid on & mechanicle layer2 active, all my boards will > space > out to proper > distance. > > Remeber, you dont need to actually fill the panel completely, just get > everything you need on the panel in the proportions you want & the PCB > manufacturer will fill out the rest of the panel to their liking. I > usually > fill close to the full width of the panel & vertically stack everything > nice. > > Good luck... > > > ______________________ > Brian Guralnick > Vergent Technologies Inc. > 438 Brahms Ave. > Dollard Des Ormeaux > Quebec, Canada > H9G 2S6 > (514) 624-4003 > [EMAIL PROTECTED] > > > ----- Original Message ----- > From: "Dusan Mihajlovic" <[EMAIL PROTECTED]> > To: "Brian Guralnick" <[EMAIL PROTECTED]>; "Protel EDA > Discussion List" <[email protected]> > Sent: Tuesday, October 17, 2006 3:24 AM > Subject: Re: [PEDA] Generating panel of PCBs in P99se is super slow... > > >> Hi, what i am interested is how the manufacturer will interpret this >> panel >> PCB. Do you have to make panel size KeepOut Layer in Step 1? Will the >> manufacturer cut the panel into smaller PCB or will they deliver the >> panel >> in >> original size? >> >> --- Brian Guralnick <[EMAIL PROTECTED]> wrote: >> >>> Ok, here we go! >>> >>> Step 1, Prep a panel PCB document, in the that PCB document, disable >>> online >>> DRC. >>> >>> Step 2, save all your different PCBs to a second stage file before you >>> copy >>> & paste it to the panel PCB. >>> >>> Step 3, on all the second stage file PCBs, in the menu ' Tools -> >>> Convert >>> -> >>> Explode Polygon To Free Primitives ' >>> Perform the 'Explode...' to all your polygon planes on the >>> PCB. >>> Step 4, under ' Design -> Netlist Manager -> Menu -> Clear All Nets... >>> '. >>> >>> Perform steps 3 & 4 for all your second stage PCB files & save them. >>> >>> Now, copy from the second stage PCB files & "paste SPECIAL (duplicate >>> designators)" into the panel PCB document as many times as you like. It >>> will paste so quickly, you can go mad. And, the Client99.exe out of >>> memory, >>> or, contineous bonging error will no longer appear. I've just managed a >>> 10 >>> megabyte PCB panel with ease... >>> >>> Good Luck! >>> >>> ______________________ >>> Brian Guralnick >>> Vergent Technology Inc. >>> [EMAIL PROTECTED] >>> >>> >>> ----- Original Message ----- >>> From: "Leo Potjewijd" <[EMAIL PROTECTED]> >>> To: "Protel EDA Discussion List" <[email protected]> >>> Sent: Monday, October 16, 2006 2:18 AM >>> Subject: Re: [PEDA] Generating panel of PCBs in P99se is super slow... >>> >>> >>> > Euhrr.... Would you care to share that trick with us? I ran into that >>> > very same problem about six weeks ago. >>> > It was not a very large panel so I put up with it, but when I need to >>> > modify it for any reason..... >>> > >>> > Leo >>> > >>> > >>> > At 16/10/06 04:34, Brian Guralnick wrote: >>> >>Never mind, I figured out how to get protel to create panels without >>> >>the >>> >>annoying "Processing pasted primitives". >>> >>It works like a dream now... >>> >> >>> >>______________________ >>> >>Brian Guralnick >>> >>Vergent Technology Inc. >>> >>[EMAIL PROTECTED] >>> >> >>> >> >>> >>----- Original Message ----- >>> >>From: "Brian Guralnick" <[EMAIL PROTECTED]> >>> >>To: "Protel EDA Discussion List" <[email protected]> >>> >>Sent: Sunday, October 15, 2006 8:42 PM >>> >>Subject: [PEDA] Generating panel of PCBs in P99se is super slow... >>> >> >>> >> >>> >> > Hi, >>> >> > >>> >> > I'm creating a large panel of smaller PCBs in P99se. The >>> >> > smaller >>> >>> >> > PCBs >>> >> > all have 3 polygon planes each. The copy & pasting is becoming >>> >> > exponetially >>> >> > slower as I add more PCBs to the panel. Right after the pastes, >>> protel >>> >> > gets >>> >> > stuck in "Processing pasted primitives". Is there a way within >>> protel >>> >> > to >>> >> > speed up, or, bypass the "Processing pasted primitives"? >>> >> > >>> >> > ______________________ >>> >> > Brian Guralnick >>> >> > Vergent Technology Inc. >>> >> > [EMAIL PROTECTED] >>> > >>> > >>> > >>> > >>> > ____________________________________________________________ >>> > You are subscribed to the PEDA discussion forum >>> > >>> > To Post messages: >>> > mailto:[email protected] >>> > >>> > Unsubscribe and Other Options: >>> > http://techservinc.com/mailman/listinfo/peda_techservinc.com >>> > >>> > Browse or Search Old Archives (2001-2004): >>> > http://www.mail-archive.com/[email protected] >>> > >>> > Browse or Search Current Archives (2004-Current): >>> > http://www.mail-archive.com/[email protected] >>> >>> >>> >>> ____________________________________________________________ >>> You are subscribed to the PEDA discussion forum >>> >>> To Post messages: >>> mailto:[email protected] >>> >>> Unsubscribe and Other Options: >>> http://techservinc.com/mailman/listinfo/peda_techservinc.com >>> >>> Browse or Search Old Archives (2001-2004): >>> http://www.mail-archive.com/[email protected] >>> >>> Browse or Search Current Archives (2004-Current): >>> http://www.mail-archive.com/[email protected] >>> >>> >> >> >> __________________________________________________ >> Do You Yahoo!? >> Tired of spam? Yahoo! Mail has the best spam protection around >> http://mail.yahoo.com >> >> >> ____________________________________________________________ >> You are subscribed to the PEDA discussion forum >> >> To Post messages: >> mailto:[email protected] >> >> Unsubscribe and Other Options: >> http://techservinc.com/mailman/listinfo/peda_techservinc.com >> >> Browse or Search Old Archives (2001-2004): >> http://www.mail-archive.com/[email protected] >> >> Browse or Search Current Archives (2004-Current): >> http://www.mail-archive.com/[email protected] >> > > > > ____________________________________________________________ > You are subscribed to the PEDA discussion forum > > To Post messages: > mailto:[email protected] > > Unsubscribe and Other Options: > http://techservinc.com/mailman/listinfo/peda_techservinc.com > > Browse or Search Old Archives (2001-2004): > http://www.mail-archive.com/[email protected] > > Browse or Search Current Archives (2004-Current): > http://www.mail-archive.com/[email protected] > > > > ____________________________________________________________ > You are subscribed to the PEDA discussion forum > > To Post messages: > mailto:[email protected] > > Unsubscribe and Other Options: > http://techservinc.com/mailman/listinfo/peda_techservinc.com > > Browse or Search Old Archives (2001-2004): > http://www.mail-archive.com/[email protected] > > Browse or Search Current Archives (2004-Current): > http://www.mail-archive.com/[email protected] > ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
