milling a chamfer with endmill

[Quick3]

Hi everyone, I'm new here, so be nice if I'm in the wrong section or my question has been exhausted already. Trying to mill a 2.5d chamfer on a cnc mill with a ball nose end mill. Is there a canned cycle that can be programmed for this or do I have to figure out compensation line by line?
Any help would be great. Thanks...
Quick

[psychomill]

There might be a macro out there for it or just program it on a CAD/CAM. But for what its worth, its a lot of "work" and cycle time. Couldn't just use a chamfer mill?

[Geof]

Change to a chamfering tool and do your chamfer in a single pass.

One of my guys wanted to prove that he could do chamfering, with a corner radius mill I think it was, and avoid a tool change; so he wrote a macro to step down the chamfer. It worked....and took so much time the machine could do a dozen tool changes.

[BobWarfield]

Originally Posted by Geof Change to a chamfering tool and do your chamfer in a single pass. One of my guys wanted to prove that he could do chamfering, with a corner radius mill I think it was, and avoid a tool change; so he wrote a macro to step down the chamfer. It worked....and took so much time the machine could do a dozen tool changes.

How was the surface finish?

Do you ever run 4 or 5 axis just because thinks work better if the cutter can stay normal to the work?

Cheers,

BW

[Geof]

Originally Posted by BobWarfield How was the surface finish? Do you ever run 4 or 5 axis just because thinks work better if the cutter can stay normal to the work? Cheers, BW

Surface finish? Not as good as using a chamfering tool.

No we do not do 4 or 5 axis. We use the 4th axis for positioning only. All our parts are designed for 2.5 or 3 axis machining.

[BobWarfield]

That's what I would have expected, faster + better finish with a tool built for it, or, if you could position the workpiece so the tool cuts the chamfer while normal to the cut.

I do wonder if 4 and 5 axis doesn't give you those advantages too. Just an OT/academic sort of question.

Cheers,

BW

[Geof]

Originally Posted by BobWarfield ......I do wonder if 4 and 5 axis doesn't give you those advantages too. Just an OT/academic sort of question. Cheers, BW

My view on four and five axis machining is that when you have to use it, use it. If you can avoid using it, avoid using it.

It hurts my brain trying to visualize true four axis machining; just using the fourth axis to position parts for 2.5 or 3D machining on two or three sides is enough mental exercise for me. Five axis machining is entering the realm of magic.

[little bubba]

Quick3, that is what they make a cam system for.

If you are just trying to do a simple chamfer, its fricken easy to hand code, time comsuming, but easy.

Increment up in Z, over in X, run a full G3(or 2 if you insist), then repeat, but increase your radius by your X stepover, pretty easy. I hand coded one 3d part, 5 seperate intersecting radiuses, it took about 2 days with CAD, it sucked, never again.

I ran a chamfer about a month ago, 60 degree included, with a .030±.01 radius into the bore and a .06±.01 radius up onto the flat. That was ball endmill territory. If not for the radiuses, chamfer tool, zip around and done.

[Quick3]

Yeah, I just hand programmed it. But, it takes a lot of code, and is time consuming. I mean you could hand program a propellor blade given enough time, but yeah, thats why we use cam. I was hoping for a repeating pattern. Just use the intial increments, and angles, and tell it where to stop. A chamfer tool works as long as the chamfer is no bigger than the tool.

[psychomill]

A chamfer tool works as long as the chamfer is no bigger than the tool.

Get a bigger chamfer tool ...

I do wonder if 4 and 5 axis doesn't give you those advantages too. Just an OT/academic sort of question.

Yes it can. With higher feeds and better finishes. Using chamfers as an examples.... Most will have a limit to feed before finishes starts to look chattered even with multi flutes because of the diameter change in the cutter (from the "small" end to the "big end"). Picture the same operation on a 4/5 axis and using the side of an endmill or bottom of one. Programmable diameter and chip loads can be much higher while attaining good finishes. The principle is the same for draft angles and such. The same endmill can do an "infinite" number of angles. Now, I'm not saying this would replace the chamfer mill in all 4/5 axis work... it most certainly does not. But optimization and utilization is opened greatly.

[ChattaMan]

I was hoping for a repeating pattern

I'm not sure what you need to chamfer but if it's the top of a hole, try this...good old "do/while" loop.

Work out your start position and trig out your chamfer angle to get your increments. 45 degrees is easiest!!

(METRIC PROGRAMMING)
M6T1(whatever ballnose)
G0X10Y0G54S3000M13 (rapid to start pos)
G43Z10H1
#500=10 (start pos in X)
#501=0 (start pos in Z)
WHILE[#500GE-5]DO1 (start of loop which ends at Z-5)
G1X#500Y0Z#501F1000
G3I-#500
#500=#500-0.2 (increment amount in X)
#501=#501-0.2 (increment amount in Z)
END1
G0Z10M9
G53Z-100Y0
M30

Traa-Laa...one chamfered hole (took a while though!

[dertsap]

if its multiple tool changes your trying to prevent then i would say if your going to be doing any drilling on the part use a 90deg spot drill for spotting any holes and use that same tool to run your chamfer