Need Help!- Cutter Comp on a Helibore? Does it work?

[elaganis]

What is the proper way to create code for Heliboring on the Haas using cutter-comp. I’ve tried a various ways to post from MasterCAM as well as editing and I get several alarms (369, 349, 340, etc.) depending on what I do. I guess my question is what is the best way to cutter comp accurate helibores? Do I post control code (tool path does NOT compensate for tool diameter) from MasterCAM or do I post computer code (tool path DOES compensate for tool diameter-therefore tool path is smaller in size) and then enter different amounts in the offset page. Also where is the best place to insert G41 D#? I get an error no matter where it’s placed because it can’t be in a line with G02 or G03. Moving it to another line and I get a Tool too big error?? Here is an example of one code where gave me problems: (posted from masterCam as “control”):



%
O1000
( TEST )
( TOOL - 01 DIA. OFF. - 01 LENGTH - 01 DIA. - .2500 3D-CONTOUR )
G17 G40 G80 G90
T1 M6
( T1 , 1/4 ENDMILL )
S1750 M3
G0 G90 G54 X0. Y.0118
G43 H1 Z1. M08
Z.1
G1 Z0. F5.
G41 D1
G3 Y.1758 I0. J.082
Z-.01 I0. J-.164
(Start Code Above)

(End Code below)
Z-.33 I0. J-.164
I0. J-.164 F1.5
Y.0118 I0. J-.082
G40
G0 Z.25
Z1.
M09
M2
%

I entered a Diameter in the offset page as .2500 and wear at .0010 (I want to leave material on my OD)

Help?

[crabbass]

A few questions,
-You say leave matl. on the O.D? typo? or are your intentions to controll a bores size with cutter comp.
-Do you use cutter comp on your machine regularly? If so are you entering the cutters radius or diameter in the Offset page? ......Or some people use "wear comp" where programmed values are at the cutters center line and the comp value deviates from that path. Each way has it's purpose.
-Did your cam post that .NC file as is? You should have an address on the G41 line, Your controll does not know where to start.
-It looks like you deleted the long code with all the absolute values for each spiral, an alternative way,(much cleaner) is to program one arc incrementally(G91) with the z value for the helix pitch and repeat that loop however many helix's you desire untill you reach the depth.
-I will give you an example from memory, I can't remember everything so forgive me I'f I make a typo. Lets say you are using a 1/4" diameter EM and your controll is set to input the tools diameter in the offset page .2500 .0000
This should bore a hole .5" in diameter 1" deep at X 0.0 Y 0.0 with a .05" step down in Z for each revolution (helix pitch)


%
O1000
G17 G40 G80 G90
T1 M6
( T1 , 1/4 ENDMILL )
S1750 M3
G0 G90 G54 X0. Y0.
G43 H1 Z1. M08
Z.1
G01 G41 D1 Y.25 F5.
M97P1010L22(<-----local call line 1010, repeat 22 times)
(.05"pitch *22revs = 1.1")

G91 G03 Y-.5 R.25(<---returns to where it left off, )
G91 G03 Y.5 R.25 (<---cleans up flat bottom )
G90 G01 G40 X0.Y0.
GO Z1.
M09
M30

N1010 G91 G03 Y-.5 R.25 Z-.025
G91 G03 Y.5 R.25 Z-.025 (> Local Sub Routine)
M99

%



Try it out, Dont try to cut with this program, just simulate to verify the codes format, then you can dial in the helix pitch, correct radius for your hole size, etc. A nice tangent lead out arc would be reccomended in the bottom of the hole. Honestly I usually don't do it this way, my cam generates a ridiculous amount of code, the path works well, and my controll doesn't mind reading 200 blocks to do the same job. I just like the clean look and ultimate controll capability of hand code sometimes.

[elaganis]

yup my bad-(typo)...I was using wear comp to control my ID (not OD) of the bores. I was going to walk in the amount I need per hole at the machine using wear amounts entered. I've enter the tool diameter and wear in offset page based on my cam code (center of tool). And Yes we use cutter comp on our machines often however this is the first time I'm using it and on a Helibore.
I like your approach but I don't hand-code as it's prone to human error and I'm damn slow at it. I can spit out code from mastercam for anything in seconds but if it's my post that I think maybe off-or haas control to read it?

[Matt@RFR]

If you're using wear comp in mastercam, you can not have a value entered in the diameter column in the control, only in the wear column.