chamfer VS radius in the modern era

[Tmoose]

[ul]
[li][/li]
[/ul]What is common/best practice these days, when there is a possibility that a non-CNC machine tools will be used?


Some of our suppliers are still using big old machine tools like Bullard VTM etc, especially for repairs on large parts.
Naturally Others are using CNC machines, especially on smaller parts.

I have been told on that on CNC machines programming time and actually machining time for radiuses or chamfers, and even breaking transitional corners, are essentially the same amount of work/time.

But My hunch is a chamfer is still the better all-purpose detail when either will suffice, as in a low stress area or an outside corner, etc.

 

[JNieman]

Universally speaking, whether manual or CNC controlled, chamfers are much more efficient to machine.

Speaking only of EXTERNAL features:

The benefits of a chamfer is that one tool can machine MANY different sizes of chamfers at the same angle. This is truth for CNC or manual machines.

The negatives of a radius is that you either use a radius-specific cutting tool to match each radius called out, or you use a ball mill to machine-away the radius and blend it for smoothing out the scallops left. (sometimes called '3d milling' the radius) which is only practical on CNC machines. For manual machines, you're stuck with using individually sized radius cutters.

For INTERNAL features, there's almost negligible difference, as either usually requires situation-specific tool selections.

I've seen some designers call out "Unless otherwise stated, all external corners to be broken .010-.030 x 45, or R .010-.030" or some such similar note. That at least gives the manufacturer the option. Because as you said, in low stress areas, it likely does not matter.

 

[BrianE22]

You don't need a special tool to machine radii with CNC machines. It's no more difficult to program either.

I personally like the look of radii over chamfers. Burrs on the entrance and exit are less for radii over chamfers also.

 

[BrianE22]

I was thinking of turning operations for my previous post. Milling is more involved for radii.

 

[JNieman]

Good point - I was assuming milling. For radii on lathes, it'd be the same tools, most likely, and not any different than wiggling the wheels a bit differently on the manuals. I had my mind tunnel-visioned into milling as that's where the differences are significant.

OP, might want to specify which you speak of specifically, though I guess we've now touched on both milling and turning anyways.

 

[KENAT]

So as alluded to above, it depends a bit if the Chamfer/Radius is cut by the tool path or by the tool shape.

If the cutter is making the shape then chamfer still has enough advantages that it's still my go to.

If being cut with the tool path then on CNC then the difference is less significant but I still tend to go Chamfer in case the part ever goes to someone without CNC for some reason (e.g. capacity issues/machine down...) and because it should fundamentally be a bit more efficient.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[3DDave]

Getting the radius to match on an as-supplied surface is tougher. Either it isn't a round or it gouges.

A chamfer can cover a multitude of sins.

No reason there can't multiple passes with different angles to approximate a radius.

 

[dgallup]

Many radii are not very "round", particularly if they are small and you look at them with a microscope. You need to specify a controlled radius (CR symbol) if you want tangency at each end without flats or reversals. Sometimes a radius is important to function but if it's not I either specify a chamfer or rely on the general note BREAK EDGE X.XX max. No benefit in over specifying something unimportant, theoretically some one has to inspect it. Chamfers are easier to inspect.

On a side note, I've seen inspectors reject a 0.2 x 45 degree chamfer because the 45 degrees was outside the default drawing tolerance of +/-2 degrees. So I try to avoid specifying an angle as it's pretty darn hard to tell what it is on a surface only 0.28 mm long. Better to make it 0.2 x 0.2 or make the angle a reference dimension. I will use an angle if the surface is longer and the angle is doing something important like the leadin to an o-ring seal.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[pylfrm]

Tmoose,

A sufficiently loose radius tolerance will allow a chamfer. Not sure how many manufacturers will actually take advantage of this fact though. A note that specifically allows both is probably a good option.

I've seen inspectors reject a 0.2 x 45 degree chamfer because the 45 degrees was outside the default drawing tolerance of +/-2 degrees.

So have I, even when the chamfer was specified by a note. I have my doubts about whether the default angle tolerance is really meant apply in this case though.

1.8.16.1 Chamfers Specified by Note. A note may be​

used to specify 45° chamfers on perpendicular surfaces.
See Fig. 1-43. This method is used only with 45° chamfers,
as the linear value applies in either direction.

Fig. 1.43 45° Chamfer[pre]
2 X 45°
or
2 X 2[/pre]

I'm inclined to consider the two methods as equivalent, and ignore the angle tolerance. Perhaps making the angle basic would solve the problem.


pylfrm