Max Radius Callout Interpretation

[[email protected]]

Hi Everybody, I wanted to know how you all personally handle max radius callouts. I think most of us know a callout of .02 MAX R could be .0 all the way to .02 but what do most of you machine it to. Let's say it's a floor radius, do you bother adding a tool just to achieve it or leave it square? What if it is in the model with an overall profile tolerance called out to the model because it's a limited dimension print? I am just curious as to why they leave it open to some extent. I believe they want some kind of radius for strength or overall appearance but anything larger than the MAX R would cause interference. I wonder these same things with plus something minus zero callouts i.e. +.020 - .000 tolerance....why not just got to the median dim and make it + or - .01 considering most machinist would shoot for nominal of the tolerance? I always felt if they call MAX R they want some kind of radius or they wouldn't have labeled it as such same with plus something minus zero callouts. It just seems to me there must be some Industry standard logic to this but I mostly just find arguments on forums.....Please shed some knowledge and wisdom anyone

[Leon82]

I make it sharp unless it's so big that it is advantageous to use a radius.

Although places.like Sikorsky have the UOS rad callouts

[Colin Gilchrist]

For me, it somewhat depends on if there is an advantage to producing the radius, or a hindrance. For external Radii, on a Milled or Turned Part, the "max 0.02R", would be a great opportunity to break the edge on the machine. This allows you to avoid having to hand-deburr the part when done correctly.

If that is the reason I'm breaking the edge, then I shoot for the median of the tolerance zone, so on a 0.02R Max, this would be a 0.010 radius for deburr purposes.

But you also have to be careful when given a print, to be sure the dimensions are coming from the theoretical "sharp corner", or the tangent edge of a fillet. I've been burned on that one badly before. When in doubt; get the answer in writing! Even an email acknowledging the question was asked, and an answer was given, can save your behind later on.

Now, on an "internal floor radius", I would typically make the floor/wall intersection a sharp corner, unless I've already got a Bull Endmill with that small of a corner radius specified. Basically; by using a sharp corner tool, or an existing tool with a small fillet (below the Max. Rad Callout), can I avoid adding another tool to my tool magazine?

Internally; I tend to ignore this (do not treat it as "the maximum of a necessary bilateral tolerance"). Whatever you do: do not let your Inspector bully you into treating this as a "required feature". Anything "Optional" is just that; not necessary to make the part in-tolerance, but may be used to your advantage, if there is a benefit to be gained. (See above about the option to deburr the part on the machine.)

 

[huskermcdoogle]

Another thing to toss into this...

Sometimes when they say .020r Max.  They may have an obscure spec called on the drawing by reference that would also allow a 45 degree chamfer that would meet the radius where they become tangent.  If you see a bunch of code specs in the title block, and you are making parts for the end customer.  It always pays to get a copy of thsoe specs so you can interpret the meaning of .020 MAX.    At one company I worked for, we had a lot of 50 degree max callouts on faced shoulders.  They were modeled at 90 or vertical.  Most of our plants would just use a shoulder mill and be done with it, and then would complain they had to deburr the edge or weren't getting very good too life.  I got clarification from engineering and used a 45 degree cutter which greatly reduced my tool cost, performance, time in cut, as well as eliminated the burr!

Notes like that on drawings are game changers sometimes.