Cutter Comp Problems

[JWB_Machining]

Hey, I'm new to using CNC machines and I'm working with a Haas TL-1 and TM-1. For now I'm just doing various random things to get aquanted with the machines.

I used IPS to mill out a circle with a Diameter of 1". Because My Tool Offsets are right due to probing the circle came out to be 1". When My tool offset was set to have a tool diam. of 0 the circle came out to be 1" plus the tool diameter. I was wondering if anyone could elaborate on how the machine does cutter comp through IPS when there is no G41 or G42 in the actual code.

Now for my coding problem. I went to mill down the side of a 1/4" aluminum plate using a carbide endmill. I set this up through visual quick code. When I ran this is it did not do the automatic compensation that IPS did. So I tried to add G41, because I'm climb milling but I keep gettin an error that I'm entering it wrong. My Set up is a carbide endmill with a Diam of 0.3114" and I want to mill down the left side of the plate starting from the end closest to me and going back to the end furthest away.

Here is the code generated by IPS, If someone could tell me where and how to put in the cutter compensation code that would be great. Also information on Feeds and speeds is also welcome. As you can see I made the depth of the cut 0.28 incase the plate is a lil thicker than 1/4"

T2 M06;
G00 G90 G54 X0. Y-3.5;
S4000 M03;
G43 H02 Z1 M08;
G01 Z-0.28 F20;
G01 Y0.3 F10;
G00 Z1 M09;
G28 G91 Z0 M05;

I Tried This and other variations but none worked, what am I missing?

T2 M06;
G00 G90 G54 X0. Y-3.5;
S4000 M03;
G41 G01 X-1.0 Y.4.6 D0.3114
G43 H02 Z1 M08;
G01 Z-0.28 F20;
G01 Y0.3 F10;
G00 Z1 M09;
G28 G91 Z0 M05;

[Geof]

Originally Posted by JWB_Machining G41 G01 X-1.0 Y.4.6 D0.3114

There is one problem: The D in the line commanding cutter compensation should be D1, D2, or any number corresponding to the diameter entered into the diameter compensation table.

Normally for tool 1 you would enter the diameter of the tool, 0.3114, into line 1 of the tool compensation page under diameter compensation. Then your command is;

G41 D01 X-1. Y4.6

You do not have to use D01 for tool 1, you can use any number but it is safer to stick with the tool number.

You can use different tool diameters for the same tool, and neither of them have to be the real tool diameter.

If you start coding properly and not using the silly Haas IPS I might be able to help with tool comp on the lathe but I only hand code.

[The White Fox]

To elaberate what "Geof" said above, this is what I'd write:

(Mill Width)
(5/16 HSS Rough EM .3125)
T5 M06
G54 G90
M03 S6750
G00 X0. Y-4.0
G43 H05 G00 Z3.
M08
G00 Z0.1
G01 G41 Y-3.75 D05 F150.
G01 X0. Y-3.5
G01 Z-.28
G01 Y.25 F60.
G01 Z0.1 F300.
G40 G91 Y.25
M09 G90
G00 Z10.

My Offset page would have Cutter Comp #5 0.1563 0.0100

I like to use the cutter comp and "wear", cutter comp for just tool size and "wear" for any additional comp like .01 from the rougher for the finish end mill to take off.
The first 9 lines or so (operation description, type of tool, . . . M8) is a standard format I use for all tools. I like to rapid during height offset to 3.0 inches above the part, so I can verify my tool being touched off with a 1-2-3 block. As you can maybe tell, I also run a Haas; a 1999 VF9.
Hope this helps.

[MikeOD]

Originally Posted by JWB_Machining I used IPS to mill out a circle with a Diameter of 1". Because My Tool Offsets are right due to probing the circle came out to be 1". When My tool offset was set to have a tool diam. of 0 the circle came out to be 1" plus the tool diameter. I was wondering if anyone could elaborate on how the machine does cutter comp through IPS when there is no G41 or G42 in the actual code.

If IPS created G12 or G13 code (which I suspect it did), then the control will use cutter comp without G41 or G42. If you look in the manual you will see how this works. You can use G12 and G13 with and without comp...but it's all done internal to the G12 or G13 code.