On 04:36 AM 16/03/2003, Dennis Saputelli said:
do you really mean '2.4mm rout'
not '2.54mm route' ?

Dennis,
A standard router bit in use on most PCB makers I know is 2.4mm (not 2.54mm). This is a good tool to use as it supports a good feed rate - much smaller and the bits break if the material feed rate is too high - according to PCB production engineers I have spoken to. I have been told that to rout out a board with a 1.2 mm or 1mm tool will be more expensive as the time to rout is longer as the feedrate is lower. There is also the risk of breakage and maybe the smaller tool becomes dull faster. I do not know how much more expensive though. I am not sure but I think I was also told once that boards could be routed in a stack with the larger tools.


The main issue I have with this tool size is internal corners have a 1.2mm radius. This can be a problem when you have to fit into a decimal pointed housing. I usually solve this by pushing the router into the PCB a small distance at a 45 degree angle to the rout edges (does this make sense?). I have figured in the past that a 0.5mm travel into the PCB at such an internal corner is enough to ensure the PCB can fit into a square edge housing. I am not being clear here I know. A picture would be much better, I know. So here it is:
http://www.considered.com.au/images/SqCornerRoutAndBreakoffTab1.gif


Also, as part of the original discussion on this subject here is a complete panel showing one fully designed board and the details of the full production panel, including routs and step and repeat (simple in this case). This board is quite interesting - the mechanics where more exhausting than the trackwork.

Here is the board and panel:
http://www.considered.com.au/images/SqCornerRoutAndBreakoffTab1.gif

And here is a photo of a portion of the final assembly, showing the dags from the breakoff and the effect of pushing the router in at the corners:
http://www.considered.com.au/images/FinalBoard1.jpg


I would like to improve the breakoff to get rid of the dags but not at too much expense of the PCB rout area - I suspect I could place a larger hole in these locations and that would do it. But it has not been sufficiently bothersome to work on it any more. Anyone got a suggestion?

I have at times specified a small router bit in a few specific places where a thin slot was used. But I pretty much always specify a 2.4mm dia tool if I am laying up a panel and need to show the rout gap. I have been told at one stage that it maybe better to make a slightly larger gap between the boards that the 2.4mm distance to allow the rout bit to be fed against the spin on all "dress" edges - that is edge of boards rather than tooling strips. This gives a better finish I gather.

I pretty much try and do what the PCB makers tell me, I am no expert. I really only get into this as we have found that it is most reliable for us to lay up the full production panel, on final production boards that is, rather than leave it to someone else.

this is of course a pain for design, so we draw everything at 0.100" and
they either joggle the bit or use an actual 0.100 bit

I find that it is pretty easy to lay up a full panel. I make liberal use of construction tracks, little track segments 2.4mm long that I con drop down and then snap to.



anyway, i have been thinking about going to 0.050 router bit width
do you have any comments on the ups and downs of that?

If it was me I would speak to the PCB makers you usually use and discuss $ vs feedrate. Maybe it is not such an issue these days. Bits may be better or fancier routing machines may be able to keep the cost down some other way.



are the router bits too thin and breakable or whatever ?
(062 thick bds)

So I have been told.



i have a board where it would actually save an appreciable amount of
material

This is an issue. Using up panel space for rout gaps vs more PCBs per panel. Take into account the (possibly) lower feedrate, and number of boards that can be routed in a stack - which ends up cheaper? PCB makers are the bods to ask that.



also regarding your breakaway holes
we have been fiddling with those for some time
(the size, count and arrangement)
but we always seem to get little 'tits' where the breakaway occurs
these are small sharp protrusions that in some cases need to be cleaned
up

I have also been playing with these over the years. I have pretty much settled on a shallow arc arrangement that "bites" into the PCB area - I am trying to get the breakoff to occur within my board area so the dags (your 'tits') are within the allowable board space. This does cost a little PCB area of course. I have experimented with holes placed so that the rout breaks into the end holes. My current design ends with two small dags at each end of the break off tab that project just beyond the desired line of the PCB. This seems to be a reasonable compromise between wasting PCB routing and placement space and clean up. In most cases we don't specify any cleanup of the edges.



i see that you (Ian) use .029 holes
we use holes more like 0.020 - 0.022 spaced pretty close
AND NON-THRU PLATED!
(else the little plating barrels can be an electrical hazard as they
detach)

Yes yes yes - definitely unplated holes. Personally, I find it easiest to use a hole you don't use anywhere else so they are easily globally selected and also simple to refer to in manufacturing notes.



also on a related topic
anyone have a feel for a reasonable design tolerance for the location of
V grooves?
i know they are a bit sloppier than routing
but they are attractive in certain cases

According to one PCB maker we use, their spec is: V-groove (center of V to nearest feature) 0.032" (0.8mm)

http://www.entechgroup.net/epc2.html - see point 7.

Dunno, if this is conservative or pretty normal. It has to include tolerance as well as the V-groove angle. I guess this would increase for thick boards.

(Hey, I just noted that they specify a 2mm rout bit as standard. So maybe I could go to a smaller tool as standard. I am not sure it would make thinghs much cheaper though.)

I actually find a lot of this stuff quite interesting and useful. I have had comments from PCB makers that they appreciate the effort I try to go to consider the manufacturing processes. I have never done a study to see if this saves my clients any money though.

Bye for now,
Ian



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to