Hi Brad, thanks for your informative email. I figured asymmetry might be a bad thing, and it turns out i don't need to board to be exactly .063". i am waiting to hear back from the fabricator as to the thicknesses of core and prepreg they stock.
thanks again for taking the time to provide me with some useful information. -rimas At 05:44 PM 8/1/2002 -0700, you wrote: >Rimas, > have just a few minutes here to type out a reply, here are my brief >comments. > >Your stackup is assymetrical. Your laminate top and bottom should be equal. >An assymmetrical stackup will usually result in unacceptable bow & twist. >Your bottom laminate thickness should match the top 6.3 mil thickness. > >Secondly, I would be pretty sure that you can't get core/prepreg in those >precise thicknesses. I don't deal with this a lot but I would be suspicious >about your xx.x mil thicknesses. Have you asked the fabricator what >core/prepreg thicknesses they stock? Use their standard cores/prepregs to >determine the best stackups, then calculate the impedance control trace >widths that you would use/need for your particular impedance. > >Third, in your stackup you did not account for copper thickness for your >total stackup thickness. 1/2 oz. CU = 0.7 mil 1 oz. Cu = 1.4mil 2 oz. Cu = >2.8mil. > > Is the thickness of your PCB that critical? Could you get away with >0.055", 0.065", 0.050" or something inbetween. Just asking because that >would give you more leeway in prepreg and core thickness selection. > > Got to run right now. Chat with your fabricator to make sure your >core/prepreg thickness is OK and that they believe your stackup is OK to >fab. Doesn't matter what stackup you create if the fabricator doesn't have >those prepregs or cores to build it with. > >Sincerely, >Brad Velander. > >Lead PCB Designer >Norsat International Inc. >Microwave Products >Tel (604) 292-9089 (direct line) >Fax (604) 292-9010 >email: [EMAIL PROTECTED] >http://www.norsat.com > > >-----Original Message----- >From: rimas [mailto:[EMAIL PROTECTED]] >Sent: Thursday, August 01, 2002 4:06 PM >To: Protel EDA Forum >Subject: [PEDA] question about layer stackup/controlled impedance >traces... > > >hello out there, > >i'm about to have my first PCB design involving controlled impedance traces >manufactured in the near future (just a small run of protos). I only have >controlled impedance traces on the top layer. using the transmission line >impedance calculation tool at: > >http://www.eskimo.com/~ultra/calc.htm > >(which someone on this list pointed me to before, thanks!) > >i've discovered that if I'm using FR4 and 7 mil traces with 2oz of copper, >that a dielectric width of 6.3 mils will give me a reasonably close >impedance (52.6 ohms and i'm aiming to get 50) > >now here's my question - is this a reasonable way to do the layer stackup? >(oh yeah, this is a 6 layer board and i'd like the resulting board to be >.063" wide) > >(TOP) >core -> 6.3 mils >prepreg -> 12.6 mils >core -> 12.6 mils >prepreg -> 12.6 mils >core -> 18.9 mils >(BOTTOM) > >this seems logical to me but being as that i am inexperienced and such >things and have noone knowledgeable around here to ask i thought i would >ask for this group's wisdom. thanks for any help, hope the >non-directly-protel related question doesn't bother anyone. > >-rimas > > >************************************************************************ >* Tracking #: A050A66B34F2154BAF06DE47FD1ACB3A65DE569F >* >************************************************************************ * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[email protected] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
