Need Help!- Cutter comp with threadmills

[PinMan]

Hey guys,

Im having an issue using cutter comp for a threadmill in a 1"-8 internal thread. Using Fanuc 0-MD control and I know that my comp lead-in needs to be equal or greater that my D Word value in my geometry offset page. Control alarms out if my lead-in is less than my D value.

Here is my problem tho: Using a .620 threadmill with an 8 pitch. My hole is .875 for my threads. I dont have enough room in the hole to have a .310 lead-in.

Any help is appreciated.

[beege]

Try and use centerline programming instead of profile programming, that way you can start out with a zero offset and adjust from there. I haven't threadmilled before, so I don't know the specifics, but if your PROGRAM comensates for the cutter diameter, then your TABLE doesn't have to.

If your hole is .875 and your tool diameter is .620, then there is .1275 from the tool edge to the hole surface. So:

G01G41G91D01X.1275F5.

will get you to the wall surface with the edge of the tool, and a programmed radius of .1275 will interpolate the hole wall, and you don't have to have a beginning radius in the comp table.

Helps?

[PinMan]

Originally Posted by beege If your hole is .875 and your tool diameter is .620, then there is .1275 from the tool edge to the hole surface. So: G01G41G91D01X.1275F5.

The only problem with that is the lead-in.
It would have to look like this:

G01G41G91D01X.310F5.

And I cant do that because of my D value, my D01 value is .310. I am currently trying to figure out a way to 'lie' to the control for the tool radius lol.

Threadmills aren't new so I am still searching for a fix

[beege]

I'm trying to tell you your D01 value CAN be set to zero to start out with, and your lead in very short, programming where the CENTER of the tool will travel. Right now, the program and offset are for the EDGE of the tool. The center of the tool wil be travelling with a programmed radius of about R.195 while threadmilling, and your lead in doesn't have to be .310

[stevo1]

Your lead in should be pilot radius - tool radius


Try this (no tool geometry in your offsets). This is using your numbers for pilot hole and tool diameter.

Pilot hole radius=.4375
Tool radius=.31
Radius to spin minus hole radius=.0625
Lead in is pilot hole radius minus your threadmill radius=.1275
Pitch to Z movement is 1/8=.125
1/4 pitch to Z movement=.125/4=.03125
Hole depth=.5

G0G90X0Y0Z3.0
Z-.5
G91G1X[.4375+.0625-.31-.1275]Y-.1275
G3X.1275Y.1275J.1275Z.03125
G3X0Y0I-[.4375+.0625-.31]Z.125
G3X-.1275Y.1275I-.1275Z.03125
G90G1X0Y0
Z3.0

This works. Becarful I did not mistype. I had to conevert it to hard numbers from the bolt circle macro that I wrote. The one I wrote will pick out in the radius what ever you specify for a pick and does as many holes as you want. I also do run with a tool radius in the offset page but I pick it up using the offset parameter value and build it into the macro. But this is the meat that actually spins. Good luck.

Stevo

[stevo1]

Originally Posted by PinMan G01G41G91D01X.310F5.

Beege is right. You are in a G91 state you can not move over X.31 from the center of the hole. you only have .1275 from the edge of your thread mill to the side of hole.

Stevo

[PinMan]

Ok, I misunderstood you beege. My apologies.

I will definately try that out, Stevo. Will let you know how it works out for me.

[ChattaMan]

PinMan.....

Use this macro for all parrallel internal threads. I set a parameter (Fanuc O-MD) to call it with G114. If you don't know how to do that, call the sub with G65 P9017. I always program in metric so your TPI will have to be converted to pitch.
To cut your thread your prog will look like this....(YOU DO THE CONVERSION FOR IMPERIAL)

O0001(1"-8 INT)
M6T1(.620 THREADMILL)
G10L10P21R7.874
G0X0Y0G54S2500M13
G43Z10H1
G65 P9017 X0. Y0. I12.7 D21. Z-15. R0. Q3.175 F400.
M9
G53Z0Y0
M30


O9017(G114 THREADMILL MACRO)
(X = X POSITION)
(Y = Y POSITION)
(I = HOLE RADIUS)
(D = TOOL OFFSET No.)
(Z = Z DEPTH)
(R = R PLANE)
(Q = PITCH)
(F = FEED)
#8=#4003(G90/G91)
#1=#5003(PRESENT Z POS.)
#5=[#4-#[#7+11000]](RADIUS TO CUT)
#28=#17/8
#29=#26+#28
#30=#29+#28+#17
#6=#5/2
G90G40G0X#24Y#25(RAPID TO X,Y POSITION)
G0Z#18
G1Z#26F[#9*5](PLUNGE TO DEPTH)
G1X[#24+#6]Y[#25-#6]
G3X[#24+#5]Y#25Z#29R#6F#9 (ROLL ON)
G3I-#5Z[#29+#17](MOVE ONE REV UP)
G3X[#24+#6]Y[#25+#6]Z#30R#6 (ROLL OFF)
G1X#24Y#25F[#9*5] (OFF TO X,Y POS)
G0G90Z[#1](RAPID TO INITIAL)
G[#8](G CODE BACK TO PREV. G90/91)
M99

[PinMan]

Thanks a ton. This is a great help!

[dcoupar]

I guess I just don't see what the problem is. If you start on center, you've got 0.500 in any direction to lead in. If your D value is 0.310, you've got 0.190 to spare. You can use either centerline or part-profile, there's plenty of room.

Position to center, feed to start depth, then:

G01 G91 G41 X0.5 F10. (ACTIVATE COMP, FEED 0.5" IN X)
G03 I-0.5 Z0.125 (HELIX 0.5" R, 0.125 IN Z)
G01 G40 X-0.5 (CANCEL COMP, FEED -0.5" IN X)
G00 Z0.1

[PinMan]

Originally Posted by dcoupar I guess I just don't see what the problem is. If you start on center, you've got 0.500 in any direction to lead in. If your D value is 0.310, you've got 0.190 to spare. You can use either centerline or part-profile, there's plenty of room. Position to center, feed to start depth, then: G01 G91 G41 X0.5 F10. (ACTIVATE COMP, FEED 0.5" IN X) G03 I-0.5 Z0.125 (HELIX 0.5" R, 0.125 IN Z) G01 G40 X-0.5 (CANCEL COMP, FEED -0.5" IN X) G00 Z0.1

You arent taking into account that my tool diameter is .620. If im in the center of the hole and feed X.5 then the edge of my tool is now at X.810. I hope this helped you.

[beege]

Originally Posted by PinMan You arent taking into account that my tool diameter is .620. If im in the center of the hole and feed X.5 then the edge of my tool is now at X.810. I hope this helped you.

He IS taking it into account, and so does your control!

If you assume X0Y0 as you hole centerline, and you have .310 in offset D1

G01X0Y0

Puts your tool in the center of the hole.

G41D1X.5, the control will put the center of the tool at .5 minus the .310 that's in the offset, or .190 (cutter COMPENSATION). Now the EDGE of the tool is at .5, if the circle is going to be milled in a counterclockwise direction.

Of course if you are going to interpolate the circle clockwise, the G41 will compensate to X.5 plus .310, because G41 tells the control to compensate to the LEFT of the geometry. That puts your tool center at X.810, and the edge of the tool at 1.120 (most likely breaking it and ruining your part)

Hope I've not confused you TOO much!