Milling a hole

[igorko]

Dear All,

My newbie question is about G41, G42

Is it possible to mill a hole 8.4 mm in diameter with 6.5 mm endmill using G41 (G42)?
The hole is 20 mm deep.
If so, could you, please give the sample code.

I am using FANUC-OM control.

Thank you very much in advance.

Yours, Igor Kozlov

[Jennifer]

Igor -

I really don't see how you could do this...the diameter of the tool is too large. You'd need to use a tool whose diameter is less than half the size of the hole (when you enable the G41 (or G42) the tool will step out the distance of the radius).

Maybe someone else has an idea?

Jen

[HuFlungDung]

You don't have to use full tool radius comp, you can use wear comp instead. This means program the toolpath at the proper offset for a given tool, and then use compensation for tweaking the exact diameter you get after you trial cut it.

The amount of tool movement when the wear comp amount is applied is not large, and the approach should easily fit inside that hole (with enough magnification to see what you are doing

[Mortek]

Many of us are used to drawing an offset ourselves, confusing the issue here. Using cutter comp your toolpath would be, if drawn, the actual outline of the hole. Thus the machine would do the offsetting meaning the cutter would only move over the size of it's radius, allowing it to still easily fit inside of the 8.2 mm hole. Yes it could be done very easily.

[CAMmando]

What he said ...

.2559 inch dia end mill cutting .31496 inch dia hole.

%
O0001 (MILL HOLE INCH UNITS)
G90 G17 G40 G49 G80
(CONTOUR)
T1 M6
G0 G54 X0. Y0. S1000 M3
G43 H1 Z2. /M8
Z.1
G1 Z-.196 F.5
G41 D1 X-.0295 F1.
G3 X.0295 I.0295 J0.
X-.0295 I-.0295 J0.
G1 G40 X0.
Z-.392 F.5
G41 D1 X-.0295 F1.
G3 X.0295 I.0295 J0.
X-.0295 I-.0295 J0.
G1 G40 X0.
Z-.588 F.5
G41 D1 X-.0295 F1.
G3 X.0295 I.0295 J0.
X-.0295 I-.0295 J0.
G1 G40 X0.
Z-.784 F.5
G41 D1 X-.0295 F1.
G3 X.0295 I.0295 J0.
X-.0295 I-.0295 J0.
G1 G40 X0.
G0 Z2.
G91 G28 Z0. M9
M30
%

CAM teh "metricschmetric"

You could also use helical interpolation (G3/G2 with a Z value).

[Mortek]

Proof is in the pudding, good job Commando.

[HuFlungDung]

Originally posted by Mortek Many of us are used to drawing an offset ourselves, confusing the issue here. Using cutter comp your toolpath would be, if drawn, the actual outline of the hole. Thus the machine would do the offsetting meaning the cutter would only move over the size of it's radius, allowing it to still easily fit inside of the 8.2 mm hole. Yes it could be done very easily.

No room for an approach that way, is there Mortek? I think that is what Jen was thinking, too. There is no room for full cutter radius comp to be applied unless you can do it before the tool enters the hole.

[Mortek]

Plunge center of hole and move out to toolpath, try backplotting commando's code and you will see. So yes a very small approach, one would have to be careful if hand programming this.

[HuFlungDung]

CAMmando's code is using a small radius toolpath which is an offset path from the hole circumference. At least that is what I see.

[wms]

HU,

From what I see, Cammando's D1 offset value would be 0.

He has taken the difference between the hole diameter and the tool diameter, divided by two and that equals the x-.0295.

[Rekd]

From what I see, Cammando's D1 offset value would be 0. He has taken the difference between the hole diameter and the tool diameter, divided by two and that equals the x-.0295.

Correct. I program exclusively this way. It will work, just use 0.0 for your CRC, unless you're using a re-grind or it's a tight tolerance, in which case go + a bit then cut, measure, adjust and cut again.

'Rekd

[HuFlungDung]

Originally posted by Mortek Many of us are used to drawing an offset ourselves, confusing the issue here. Using cutter comp your toolpath would be, if drawn, the actual outline of the hole. Thus the machine would do the offsetting meaning the cutter would only move over the size of it's radius, allowing it to still easily fit inside of the 8.2 mm hole. Yes it could be done very easily.

Yes, Ward, I know. But Mortek seems to be saying that the toolpath would be the actual outline of the hole, and I'm saying it isn't.