Cutter Comp Activation question

[bigalexe]

Ok let me first say i am in BEGINNING CNC class.

My teacher stated i need two right angle movements to turn on Cutter Compensation so i get something like the following

(Cutter above the part)
N120 G41 Z-.04 F12.
N130 X2.5
N140 Y2.5
(Ok so now we get cutter compensation YAY!)

Now to my question. My teacher stated the movements must be greater than the diameter of the cutter, I'll use a 3/4" Endmill for the example here. So does that mean the Cutter itself needs to move 3/4" in total or i need to program at least 3/4" of movement into the code?

So lets assume the cutter is at position (0,0)
We call the G41 code for left side comp.
Do i need to program the cutter to go to (1.125,0) then (1.125,1.5) thus moving the cutter centerpoint a full cutter diameter. or can i just go (0.75,0) then (0.75,0.75) thus moving the cutter only .375 because the cutter moves to the left of the path?

[gsrmmeza]

NO and NO
You do not need two right angle moves to go into cutter comp. All you need is a linear move ( a straight line ). It can be done on arcs with the Fadal but it is not wise to do that in case you transfer programs to different machine manufacturers. Some are real picky on how cutter comp can be done. Here is a sample program to trim the left side of a 2 inch part.

TA,1
%
N1O1* SAMPLE PROGRAM TO TRIM PART
N2* X0 LEFT Y0 FRONT Z0 TOP OF PART
N3* T1 .750 ENDMILL
N4M6T1 ( CALL UP T1 )
N5M3S1390 ( TURN ON SPINDLE )
N6X-.375Y-.4G8E1 ( POSITION TO CUT LOCATION )
N7H1Z.1M7 ( TOOL LENGTH AND COOLANT )
N8G1Z-.5F35. ( FEED DOWN IN THE "Z" )
N9G41Y-.3F20. ( GO INTO CUTTER COMP ) ***NOTICE .1 SHIFT***
N10Y2.3 ( TRIM LEFT SIDE )
N11G40Y2.4 ( CANCEL CUTTER COMP ) *** NOTICE .1 SHIFT***
N12G0Z3. ( RAPID UP )
N13M5M9 ( COOLANT AND SPINDLE OFF )
N14X0Y0E0 ( G0 TO PART CHANGE POSITION )
N15G49Z0 ( CANCEL TOOL LENGTH )
N16M1 ( OPTIONAL STOP )
N17M6T1 ( CALL UP T1 )
N18M2 ( END OF PROGRAM )
%

Your sample shows you attempting cutter comp in a down "Z" move I have never seen this. I don't even know if it would work. I have cancelled cutter comp going up in the "Z" ( ex: G0Z.1G40 ) But like stated above some machine don't like that.

Your second question as to how much you need to move to go into cutter comp. I have done moves as small as .003 for a 1/16 endmill to as large as 1.500 for a 1/2 endmill it depends on what you are trying to do. The majority of the time I shift .100 and it doesn't matter if the cutter is .0625 or 1.250
Why have a bunch of unnecessary motion when you don't need it.

[3axisrookie]

I turn on comp in my e1 line and feed it fast. Very easy on fadal. And cancel in my z1. move. I also have to agree comp won't work with a plunge move.

I was taught the fanuc way too. 90 degree move and more than half the cutter radius. None of that is needed on fadal.

Just write a few programs and look what you programmed and the actual absolute position to see how it all works.

[little bubba]

BigAlexe, your instructor is an idiot.

Gsrmmeza is correct on what he is showing you, however he is running wear comp (programming to the center of the tool), which I prefer. This allows you to have very small lead ins.

You instructor is trying to get you to program to the part, which is a lot easier to do when hand coding. As for TWO right angle moves, no, you don't need that, you just need some sort of linear move (Fadals will turn on comp on an arc, not suggested as has already been said). When hand coding a single perpendicular move is easiest to code. And it only has to be bigger than the radius of whatever is in your tool offset, it really has nothing to do with the actual tool. Which brings you back to wear comp, where your diameter/radius offset may only be .002 or .003 or even zero, or negative, so you only need a very very small lead in.

What your instructor is trying to get you to do just seems cumbersome and confusing.

[bigalexe]

ok sorry about putting the G41 code in the Z axis line, i didnt mean to do that it was late for me.

So let me just confirm that according to what you are saying I only need 1 move after my G41 code and NOT 2.

My teacher is trying to teach this in relation to hand coding and im just curious about it. We start on Mastercam next Monday but i like hand coding because its challenging, id never use it in practice i just like it.

[little bubba]

Originally Posted by bigalexe ok sorry about putting the G41 code in the Z axis line, i didnt mean to do that it was late for me. So let me just confirm that according to what you are saying I only need 1 move after my G41 code and NOT 2. My teacher is trying to teach this in relation to hand coding and im just curious about it. We start on Mastercam next Monday but i like hand coding because its challenging, id never use it in practice i just like it.

BigAlexe, after a nice hard 16 hours of crawling around in a machine and just reading your post, I know what your instructor is telling you and why, but its still confusing, or since you are new at this, you aren't completely understanding what he is saying yet.

He is trying to get you to program to the part.

Example. You have a piece of stock in the vise, you want to bring it to length, its one inch in the Y. XY zero at the top right corner. You are hand coding to part dimensions, which is a good idea. So you need to cut from 0,-1 to 0,0.

He wants you to code, 1/2" endmill.

G0 X -.3 y-1.3 Speed, feed, get to your Z height and all that.
G41 Dxx X0. <--- first perp move
G1 Y-1. <--- second perp move to get to part dim. not needed.
G1 Y0 <--- another move to part dim, not needed.
G1 Y.3
G43 X-.3
on to the next thing.

[carbidecraters]

LOL looking at that second program posted in this thread makes me very proud of the fact the 88hs doesnt require you to turn off the spindle, turn off the coolant or turn off the tool height to change a tool.

[machinist_1]

You have to make your Z move first then turn on cutter comp. You must also turn it off before a Z move. FADAL hates a Z move with comp. turned on.

[HuFlungDung]

The reason for the 2 move lead in which Bubba alluded to in his post#6, is because in real life, when one is cutting an open profile (one that is not a closed loop or closed chain of entities), you don't want the tool comp to turn on and bring the tool immediately to the beginning of the profile because the move may be slightly inexact (due to the feed speed of the machine) and this will leave a bit of a ramp on the wall of the cut. So by adding a small amount to the length of the first entity, you'll see the tool has a chance to get into position and will come straight onto the profile and the cut will look nice and straight. Same thing goes for when the tool leaves the end of the part.

As for the length of the initial movement, the real lead-in movement, it only needs to equal the tool radius. In actual fact, there is no movement when the lead-in distance equals the tool radius, instead, this is the instant that the control reckons that instead of tool centered (on the toolpath) it switches to tool tangent. So if you use a 3/4" tool, the minimum lead in is .375" (at 90 degrees!) and produces no movement. So if you want a little bit of clearance, you can add a few thousandths to that. This is for full radius cutter comp which is most likely what the instructor wishes to teach. If you add a few thousands to the lead in/lead out length, this will permit you to go slightly larger with the tool radius in the control comp register.

A radius lead in is also suitable so long as it at least equals the tool's true radius. The limitation is that you cannot adjust the tool radius compensation wear value indiscriminantly, because if the total of the tool radius + wear > than the lead in radius, you will get a cutter interference alarm. At no time can the control compensate a radius that is smaller than the tool's radius because it is physically impossible to execute it. Some users may think that they are 'getting away with something' by using only wear comp and a zero tool radius because this reduces the incidence of interference alarms. However, the interference alarm is simply a warning that the machine cannot cut the profile to spec because it is impossible to cut it with the given parameters.

When using cutter comp on a closed profile, a single line lead-in and lead-out is typically all that is used. However, a high feedrate of the machine can still cause a little blip on the profile where the tool comps on and off the profile. So even in those circumstances, it can be advantageous to use the 2 move method in conjunction with either the entry or the exit move because this creates a small amount of overlap which smooths the profile better at the high feedrate.

Most of the time, I would imagine that people have an ideal tool radius in mind when they are programming with full radius tool comp. If you feel that you might at some time in the future, use a significantly larger tool, then all lead in distances and/or radii should be adjusted larger for the largest practicable tool that will be used.