[MCImes]

Hello all,
I need to mill a cam on into a shaft. I have never used g7.1 and am wondering if someone could post a basic cylindrical interpolation program in the x/c axis. It doesnt need to be fancy. Im milling a .170" (circular cam, constant radius) on a .250 shaft, offset from center .040.

If you have one handy I'd be curious to see a program for an increasing radius cam as well.

Thanks!

[z369]

[QUOTE=MCImes;1086424]Hello all,
I need to mill a cam on into a shaft. I have never used g7.1 and am wondering if someone could post a basic cylindrical interpolation program in the x/c axis. It doesnt need to be fancy. Im milling a .170" (circular cam, constant radius) on a .250 shaft, offset from center .040.

If you have one handy I'd be curious to see a program for an increasing radius cam as well.

Thanks!

I'm seriously not trying to offend here, but your control manual should get you on track, if all else fails run a straight up cylindrical program and just do a Y/core offset, the machine should take a .040 offset.

[gizmo_454]

I am certainly not offended. I do, however, feel MCImes' pain. Many times the books are unclear, and not many examples are in them. For someone to post a short amount of code and explain it is, many times, more helpful than a book ever could be.

:cheers:
Mike

[SirDenisNayland]

I use G107 (same thing) on my star a lot here is how I run it

M5 (stop spindle)
M8G98 (c axis on, IPM feed)
M36S3500 (live tools on)
G118 (cross tool yz interp)
G0X0Y[#531+.1]Z1.4547C-16.05T10 (position tool)
G107C.4745 (RADIUS VALUE OF YOUR CUTTING DEPTH .949/2)
G118H0.W0. (YOU NEED THIS LINE DO NOT MODIFY)
G1Y.949F5. (feed into material and start your work..)
...
...
..
G1Y1.049F100. (feed out)
G118 (must call G118 again)
G107C0. (cancel cylindrical interp)
M9 (c axis off)
M38 (live tools off)

Its really straight forward really.. all I do is I take post from a mill, and I convert the X to C, y to Z and z to Y*2 (xyz post to what you run in the star, czy.. in say a citizen where the cross tools feed towards the material in x it would be czx). Radius values in G2/G3 interps remain the same, and the interp is calculated based off of the radius value of your cutting depth you gave when you turned G107 on. Your G2's however become G3's and vice versa.

I found the manual to be really good and its how I figured it out.. Oh and by the way, no G0 rapid moves in G107. And if the machine alarms, say you put in an accidental G0 while in G107.. you must shut down the machine and restart it.. I could never figure out a way to get out of G107 mode. Anything you try to do in MDI after an alarm will come up another alarm "CANCEL G107 MODE" or something like that.. but typing G107C0. in MDI doesnt work hah. Not a huge issue, just remember to use a high feed rate move instead of rapids!

Hope this helps a little..

[z369]

I am certainly not offended. I do, however, feel MCImes' pain. Many times the books are unclear, and not many examples are in them. For someone to post a short amount of code and explain it is, many times, more helpful than a book ever could be.

:cheers:
Mike

Sorry my post was dumb.

[UK-Engineer]

Metric example from Miyano ABX - puts an equal chamfer around a cross hole

(DEBURR CROSS HOLE C AXIS )

(#100=DIAMETER OF CIRCLE)
#100=*
(#101=PRE TURNED DIAMETER)
#101=*
(#102=CENTRE OF CIRCLE)
#102=*
(#103=FEEDRATE)
#103=*
(#104=STARTING C AXIS VALUE)
#104

N*
G40G80G18
M5
M13
G28C0
G0C#104
T**** M91
G54
G97S****M43P12
G0G98Y0 Z#102 M8
X[#514+2.0] (M28)
G1 X[#101-2.0] F#103
G18W0H0
G07.1C[#101/2]
G1W-[[#100-2.0]/2]F#103
G3W[#100-2.0]C#104R[[#100-2.0]/2]
G3W-[#100-2.0]C#104R[[#100-2.0]/2]
G1Z#102
G07.1C0
G18U0W0
G0X[#514+2.0]
G28U0V0
M45
M5
G18
G99
M01

[SirDenisNayland]

I hate to break it to you UK Engineer, but that will not put an equal chamfer on a cross hole. Equal being a path such that the the centerline of the chamfermill is perpendicular to the tangent line at the point which the crosshole intersects the OD of the stock.

It makes a circular path wrapped around the diameter of the stock.

However a crosshole creates a circular path projected onto the stock, aka an ellipse when flattened.

So you need to create an elliptical path, and then wrap that around the stock if you wish to truly create a perfect crosshole deburr. However you can't use cylindrical interpolation for this. If we were simply tracing the path of the intersection it would work, but there has to be an inside offset for the cutter, and following an ellipise simply offset a certain distance won't cut it - when you get to the C axis limit the rotation axis of the cutter is NOT perpendicular to the tangent of the crosshole intersection. which means were looking a 4 axis path xyzc vs cylindrical which works off of three axis, one of them simply being your plunge axis, and the other two, ZC simply being an adaptation of a planar XY path wrapped onto a diameter. On a citizen where the plunge axis is X regardless of the orientation of the live head (vs say a star where the cross tools oriented 90 degrees to the gang plunge in Y) this means that as the C axis rotates the Y axis also sees movement as well as the Z axis. If your cutter rotation axis is perpendicular to the tangent line of the crosshole intersection as it should be, this means that when the c axis is rotated to its max position (the side of the crosshole) that the Y axis is moved over by exactly the cutter offset distance. So to do this properly we have to acknowledge that 1) we have to abandon cylindrical interpolation, and 2) even if we did just want to trace the path of the intersection and use cylindrical interp, that simple G2/G3 arcs will not suffice.

It's not so visually apparent where the radius of the crosshole is much smaller than the radius of the stock, but when the radius of the crosshole approaches the radius of the stock it becomes blatently clear.

Hypotehtically speaking for example purposes, say the crosshole radius is equal to the stock radius. We're going to need to move the C axis a full 180 degrees, or pi radians aka 3.14radians, yet if you follow your method, the C axis will only move 2 radians total - nowhere near enough, and nowhere near the point where the axis of cutter rotation approaches perpendicular to the tangeny of the crosshole intersection, even disregarding a Y offset motion.

Now, there is the question of just what is perfect? if the center of the circle in line with the cutter is C0, and we have +Z and -Z, the crosshole and the diameter form a 90 degree angle, and a 45 is 'perfect' at this point, however as we move to the +C and -C values @ Z0, the sides of the crosshole will form an acute angle with the tangent to the stock at the crosshole intersection, putting a 45 to the tangent at this point will put a much greater angle when viewed from the perspective of the crosshole, closer to a 90 degree rather than the 135 degree angle at C0, then there is how the chamfer itself cuts past the intersection point and the angle it actually creates at the stock diameter.. it is for all these reasons that it makes it even lesser apparent thats its not "perfect." Here is a very rough sketch illustrating what I mean:


If anything the best way is to avoid any C axis rotation and keep the cutter axis of rotation parallel to the crossholes axis of rotation using an XYZ path, such that a 45 is created to the actual wall of the crosshole aorund the whole hole. Or perhaps make a path such that the chamfer amount is taken into consideration and a maximum C axis value is calculated such that the angle where the chamfer meets the crosshole is equal to the angle between where the chamfer comes in contact with the OD and thus the tangent line at THAT point, rather than the crosshole intersection point, which gets cut away.

I've thought a lot about this, and perhaps ive said too much..
.02

Cheers