As with any electronic component, the design engineer needs to specify the material and tolerance. PCB material is no different in this respect. If you specify the geometry of the traces, the thickness of the dielectric
material between layers, and the electrical grade of the material used, your design should perform within the expected tolerance levels.
Leaving it up to the fab house to modify trace width in order to compensate for the dielectric variations in the laminate may result in the correct impedance, but this will also invariably alter the capacitance and inductance of
I think that one will have a greater control over the performance of a design by specifying tolerances of all components used, including the PCB laminate.
Kim Flint wrote:
> I think the guy's point was valid. Basically what he's saying is the real
> fabrication process is rather complicated, moreso than many engineers
> realize. If you want accurate results according to your design, you should
> understand their process as best you can, and also provide a complete set of
> information so that they can meet your requirement. This means being more
> explicit in the documentation you provide the fab house, and probably
> working more closely with them than a lot of engineers are likely to be used
> to. He's not saying you should let the fab house design for you, but that
> you should work with them and provide the info they need so they can
> actually produce what you designed.
> An example that comes to mind (and it's really hypothetical, I don't know
> how valid it is...): say a fab house uses several different supppliers of
> FR-4 material. Maybe they know that vendor A typically has Er=4.3, vendor B
> typically has Er=4.1, and vendor C typically has Er=3.9. If you just say you
> want 5mil dielectric thickness, they'll probably choose any of those vendors
> for you. If you happened to base all your calculations on Er=4.3, and they
> give you Er=3.9, you might have a problem. On the other hand, if you
> explicitly say you are controlling impedance with an assumed Er=4.3 in your
> calculations, they would know to choose vendor A to get what you want.
> At 10:12 AM 3/25/99 -0800, Ron Miller wrote:
> >I am appaled by this vendors remarks but not surprised.
> >We engineers design the boards and if some fab houses do not want to build them
> >as directed, or maintain the tolerances required then we will find someone
> who will.
> >The fab houses have no way of knowing that a pad size is designed to provide a
> >capacitance that is optimized and simulated to make the entire circuit work as
> >desired. They do not make differential impedance measurements for differential
> >Basically, what it boils down to is that they have been getting away with
> >adjusting their processes and even the artwork to get the impedances that
> are specified
> >because they have not been keeping their materials properties dimensions and
> >post process trace widths to the fab drawing requirements.
> >It is time for that to change. I for one will not let the PCB fab house
> design the board
> >for me.
> >Ron Miller
> >Kim Flint wrote:
> >> At the PCB West conference yesterday, during the course on Materials for
> >> High Speed Design (which was quite interesting, I wasn't familiar with
> >> much
> >> other than FR-4, but that's another topic....) a fellow in the audience
> >> happened to be from a major fab house and made some rather interesting
> >> comments that seem to pertain to your questions.
> >> One was that FR-4 material is made by a variety of vendors, and it is
> >> not
> >> all the same. A fab house will be taking those differences into account
> >> for
> >> their controlled impedance calculations, depending on the material
> >> vendor
> >> they use. This could account for differences, even if processes are
> >> supposedly equivalent otherwise. (In any case, the dielectric constant
> >> for
> >> FR-4 is not very stable and could be a signigicant source of error.)
> >> He also said about the same thing Katie said below, that different fab
> >> houses tweak their calculations according to empirical data from their
> >> particular process.
> >> Most interestingly, he said they've lately had a lot of trouble with
> >> engineers possibly knowing a little too much for their own good (or not
> >> enough :-) and trying to achieve controlled impedance just through
> >> specifying trace widths, copper weight and stackup dimensions. Since the
> >> real world of PCB fabrication is not that ideal, and all fab houses are
> >> not
> >> equal, this often results in completely wrong results on the board. And
> >> the
> >> fab house can't do anything about it since they don't really have enough
> >> info to know how to compensate their process to meet your requirement.
> >> His
> >> request to engineers was to include, in addition to stackup, trace
> >> width,
> >> etc., the impedance you are targeting, the calculations you used to
> >> determine that, and any assumptions you might have made. (i.e., Er=4.3.)
> >> This info should be *on the fab drawing*, as that is the thing that will
> >> actually get looked at during fabrication. With this data, the fab house
> >> should be able to compensate appropriately for their process, and
> >> therefore
> >> they might be able to do a better job of getting you what you want.
> >> good luck...
> >> kim
> >> At 01:51 PM 3/24/99 -0500, Laurence Michaels wrote:
> >> >Katie Rothstein wrote:
> >> >>
> >> >> Laurence,
> >> >> Just a quick thought about your question. Different board
> vendors have
> >> >> different processing capabilities (line width, total board thickness,
> >> >> size, etc.) This could be why some board shops can meet your required
> >> >> impedances and some cannot. I'm not sure exactly what you are asking
> >> about the
> >> >> different calculations, but many board houses have impedance calculation
> >> tools
> >> >> that take empiricle data to help make corrections for their own processes.
> >> >> -Katie
> >> >
> >> >It sometimes seems that, even with 'equivalent' processes, allowing the
> >> >same board thickness, size, line width, and layer stackup, board vendors
> >> >will come up with different values for trace impedance, generally
> >> >requiring them to tweak the board stackup. Since we sometimes like to
> >> >use different board vendors, even on the same board, it would be nice to
> >> >be able to specify FR4 and copper, and use only one layer stackup,
> >> >instead of having to keep track of which vendors require which different
> >> >dielectric heights. It would be even better to come up with a
> >> >theoretical calculation that works in practice, since some people seem
> >> >to think that anything should be able to be calculated without having to
> >> >add tweak factors for different vendors. I'm beginning to realize that
> >> >this is not the case.
> >> >
> >> >What I'd really like is to come up with a set of layer stackups, perhaps
> >> >including different stack heights for different vendors, for a few
> >> >different controlled impedances and numbers of layers. Doesn't seem too
> >> >likely, as even including the true dielectric constant for the specific
> >> >vendor's material in the calculation doesn't always come out within 10%
> >> >of the measured impedance. Plus I'd rather only have one layer stackup
> >> >(including diel. heights) per board, regardless of vendor. Wishful
> >> >thinking...
> >> >
> >> >I'd also like a less expensive way to measure trace impedance than a
> >> >TDR, so that we can check the board vendor's claims ourselves. Any
> >> >ideas here?
> >> >
> >> >-- Laurence
> >> >
> Kim Flint, MTS 408-752-9284
> ATI Research email@example.com
> **** To unsubscribe from si-list: send e-mail to firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****
-- Philip R. Gantt email@example.com . . Phone : (408) 527-2918 | | Fax : (408) 526-5504 ||| ||| Pager : (408) 814-8868 ||||| ||||| 170 West Tasman Drive, SJ-G2 ||||||||| ||||||||| San Jose, CA 95134-1706 (U.S.A.) .:|||||||||||||||||||||||||:.
**** To unsubscribe from si-list: send e-mail to firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****