[glenthemann]

Im apprenticing, and I was setting up a job yesterday and I took the manual home to read up on it and get the programming where I want it.

Basically, everything works the way its supposed to except for the leadout after the finish cut. The final hole diameter is 2.39", roughing out to 2.38 before the finish.

Here is my code

T1M6 (5/8 END MILL)
G90G54G0X0.0Y1.195S2400M3T2
G43Z2.0H1
G42D1F14.0
G65X1.195Y0.0
G0X0.0Y0.0
Z1.0
G2X0.0Y1.19R0.595F14. (LEAD IN)
X0.0Y-1.19R1.19
X0.0Y1.19R1.19
X0.0Y0.0R0.595 (LEAD OUT)

G2X0.0Y1.195R0.5975 (FINISH LEAD IN)
X0.0Y-1.195R1.195
X0.0Y1.195R1.195
X0.02Y1.1948R1.195 (OVERLAP)
X0.0Y0.0R0.5975 (LEAD OUT)
G65X-1.195Y0.0
G40G0Z2.

dont pay attention to the z values, those were just there so we could see the toolpath in the air above the part.

Basically everything works flawlessly until I get to the finishing lead out - rather than arc to x0y0 it seems to move linear. I tried removing the overlap section, the G65 section, both at the same time, etc and it still seems to move linearly. It doesnt make any sense because the previous lead out works the exact same and the numbers are spot on, so its not an issue of the NC thinking the radius is too large or anything. We tried a bunch of things, and something of interest to note is that if a g1x0y0 is placed after the roughing lead out line, then that lead out behaves in the exact same manner as the finishing lead out behaves; not the desired way.

Im using a 5/8" end mill, and the program starts at G54 x0y0.3125 (the compensation is perfect here), But when it does the lead out move to x0y0, with the comp still on it should be in the same place it starts..

Really confused here.

The control im using is a Milltronics centurion (I dontknow what you guys think of the machine, but we all hate it here, its so finicky and a pita.. hence this issue).

Any help would be greatly appreciated, like I said I am new, and the guy I am apprenticing off of hates cutter comp and never uses it, yet I only see advantages, but Im thinkin that perhaps this isnt a cutter comp issue at all? I want to get this to work, we do use mastercam and for the time being just used it to generate the path for the circle, but I dont feel there is any need to use mastercam for such simple things, and its the easy way out in this case, rather than actually figuring out where my syntax may be incorrect. Thats kind of the way Id like things to change in this shop, it seems guys know what works, but not HOW it works, or WHY.. which just isnt the way I work, with anything, ever, I NEED to know. For instance I am the only one in the shop who really understands a G28 command.. guy im apprenticing off of thought the values you input after g28 were where the machine moved to (ie g28y0z0, he thought it brought y to home and z to home, rahter than those values being an intermediate point before the machine returns to reference, and it just so happens our reference is home position, so thats how he thought it worked.. but I disagreed citing thebook and we did a little experiment and low and behold I was right).

Thanks

[glenthemann]

I guess I should note that G65 in this case is not a macrocall, but a "non movement".. basically what it does is it allows you to eliminate the need for a prep move prior to moving to your start position so that cutter comp is properly initiated, it eliminates the "jumping" that can occur. As im sure you all know the compensation is calculated based on the previous point, the current point and the next point.. if I just moved to x0y0, then the comp would kick in on the first circular interpolation and could cause problems when the machine "jumps" into the comped position such as ramming into the part etc.. So basically G65 gives the machine a 'previous' position to work with, even though no movement was made.. its pretty clever if you ask me.

Ive been a programmer all of my life, html, css, php, c, c++, visual basic, etc.. it goes on and on. Correct syntax is very important to me, as is elimating redundancy.. I cant stand the mentality of some people of "if it works its good enough, who cares if I dont understand why it works".

[beege]

Usually turn on comp with a XY combination (X, Y or both)
Whenever you have a series of arc moves, you can initiate those by just one "G02". But if you need to have a linear move, you MUST use a "G01" or "G00" there. G00, G01 and G02 are modal,,,, so

G00G54G90X0.0Y1.195S2400M3T2
G43Z2.0H1
G00G90G42D1X0.0Y0.0 (put it back into absolute with the G90)
Z1.0
G2X0.0Y1.19R0.595F14. (LEAD IN)
X0.0Y-1.19R1.19
X0.0Y1.19R1.19
X0.0Y0.0R0.595 (LEAD OUT)

G2X0.0Y1.195R0.5975 (FINISH LEAD IN)
X0.0Y-1.195R1.195
X0.0Y1.195R1.195
X0.02Y1.1948R1.195 (OVERLAP)
X0.0Y0.0R0.5975 (LEAD OUT)
G0Z2.
G40G91X0Y0
G90

Of course, never having programmed that particular control, some of my syntax could be off, but the idea is still there...

[ChattaMan]

.....or another way.

T1M6 (5/8 END MILL)
G90G54G0X0.0Y1.195S2400M3T2
G43Z2.0H1
G42D1F14.0
G65X1.195Y0.0
G0X0.0Y0.0
Z1.0
G2X0.0Y1.19R0.595F14. (LEAD IN)
X0.0Y-1.19R1.19
X0.0Y1.19R1.19
X0.0Y0.0R0.595 (LEAD OUT)
...
G40G0Z2.


G0 X0.0 Y0.0
G0 Z1.0
G1 G41 D1 X0.5975 Y0.5975 F14 (APPLY COMP)
G3 X0.0 Y1.195 R0.5975 (LEAD IN)
Y-1.195 R1.195
Y1.195 R1.195
X-0.5975 Y0.5975 R0.5975 (LEAD OUT)
G1 G40 X0.0 Y0.0 (COMP OFF)
G0 Z2.0

Your code in black (which you say works). My code for finish pass in red.
I don't know your control or machine.
Better to use G41 and G3 for internal and G41 G2 for external, always climb milling.
If you're wanting to learn how and why, forget the G65 block until you've learned programming the standard way. Then when you get good, use the trick stuff.
The ones that say they hate cutter comp are the ones who don't know how to use it. It will never do any "jumping" moves unless programmed wrong.
I like to apply comp after the Z move. Apply comp on a G1 or G0. Then comp off on a G1/G0, then move up in Z.
When using cutter comp try to imagine yourself as the cutter. Maybe you are driving a car but it's not got reverse gear. You can only go forwards once comp is applied. You're going down the road travelling in X+ direction. Then you'd like to go back in X-. You cant, you've got no reverse gear. You have to go to the roundabout or do a U-turn. Whilst going round the roundabout you are still travelling forwards. Once you're right round you now travel in X- direction. All the time you have been facing forwards.
With no comp it's easy... move in X+, bang it in reverse, move in X-.
Blimey...never explained it like that before. Hope it makes sense.
Forget the overlap, shouldn't really need it.

[glenthemann]

.....or another way.

T1M6 (5/8 END MILL)
G90G54G0X0.0Y1.195S2400M3T2
G43Z2.0H1
G42D1F14.0
G65X1.195Y0.0
G0X0.0Y0.0
Z1.0
G2X0.0Y1.19R0.595F14. (LEAD IN)
X0.0Y-1.19R1.19
X0.0Y1.19R1.19
X0.0Y0.0R0.595 (LEAD OUT)
...
G40G0Z2.


G0 X0.0 Y0.0
G0 Z1.0
G1 G41 D1 X0.5975 Y0.5975 F14 (APPLY COMP)
G3 X0.0 Y1.195 R0.5975 (LEAD IN)
Y-1.195 R1.195
Y1.195 R1.195
X-0.5975 Y0.5975 R0.5975 (LEAD OUT)
G1 G40 X0.0 Y0.0 (COMP OFF)
G0 Z2.0

Your code in black (which you say works). My code for finish pass in red.
I don't know your control or machine.
Better to use G41 and G3 for internal and G41 G2 for external, always climb milling.
If you're wanting to learn how and why, forget the G65 block until you've learned programming the standard way. Then when you get good, use the trick stuff.
The ones that say they hate cutter comp are the ones who don't know how to use it. It will never do any "jumping" moves unless programmed wrong.
I like to apply comp after the Z move. Apply comp on a G1 or G0. Then comp off on a G1/G0, then move up in Z.
When using cutter comp try to imagine yourself as the cutter. Maybe you are driving a car but it's not got reverse gear. You can only go forwards once comp is applied. You're going down the road travelling in X+ direction. Then you'd like to go back in X-. You cant, you've got no reverse gear. You have to go to the roundabout or do a U-turn. Whilst going round the roundabout you are still travelling forwards. Once you're right round you now travel in X- direction. All the time you have been facing forwards.
With no comp it's easy... move in X+, bang it in reverse, move in X-.
Blimey...never explained it like that before. Hope it makes sense.
Forget the overlap, shouldn't really need it.

I understand how the left and right cut aspects work, thats not an issue. My issue was that rather than arcing out of the finish cut it pretty much just moved linearly, Ill see if I can draw up a diagram later of what I mean. And I was told to conventionally cut the hole rather than climb cutting.

You say there is no "jumping".. so explain to me please how you would not have that happen?

For instance if I do the follwing with a 1 inch cutter (just a simple side mill, imagine a 2 inch piece you need to cut a step in)

my questions will be in brackets beside the lines

G90G54G0x2.0y0.0
G0G41 D1 x1.0y0.0 (will the center of the tool be at x1y0 or x1y-0.5?.. from what ive learned the tool would rapid to center being x1y0 and then "jump" to x1.0y-0.5)
G1 x-1.0
G0G40x-2.0y0.0 (will comp remain on until it reachs x-2.0y0.0, or would it instantly turn off, ram into the part and then try to rapid to position? And if it does remain on until that point, what happens when it reaches x-2.0y0.0? It must reset itself, so the tool must jump in the positive y direction by half an inch no? Or does it slowly ease off the comp linearly until it reaches that point, also possibly hitting the edge of the part?
G0Z2

Those are little things I guess I dont quite understand and when I read about G65 in the book it solved all those dilemmas in my head, but like you said its machine specific and I do need to know how to program other machines like our haas and matsurra. I assume the way the machines apply their comp is also pretty specific so one method may not work for all?

What I dont get about turning the comp on and off is really the jump thing, you say if you program it right there should be no jump.. but if I am at x0y0 with cutter comp on and I turn it off, the machine wants the center of the tool at x0y0, so in essence it HAS to jump, doesnt it?

The main reason the guy at my work hates cutter comp is because of the jumping aspect and the fact that you have to do much more work to get something cut, leading in moves, leading out moves, pretty much more moves which waste time, and in a production environment such as ours time is money. Although being able to throw in different sized cutters and adjust diameters for wear on the fly is a lot easier than editing hard-code, so I guess its a bit of a trade off.

In any case, I want to learn comp properly, and apply it to all the jobs I set up.

Thanks for the responses

[ChattaMan]

G90G54G0x2.0y0.0
G0G41 D1 x1.0y0.0
G1 x-1.0
G0G40x-2.0y0.0

To do this you need to approach it from the side, not the end.

This will climb mill....and will not "jump"
G90G54G0x2.0y-1.0
G0G41 D1 y0.0(cutter C/L will now be at x2.0 y-0.5)
G1 x-1.0
G0G40y-1.0

I agree using comp does mean more moves leading on and off the job. Don't use it on the simple parts. When it comes to profiling though, you just program the sizes off the drawing rather than having to work out the tool stand-off amount.

.........................................

What I dont get about turning the comp on and off is really the jump thing, you say if you program it right there should be no jump.. but if I am at x0y0 with cutter comp on and I turn it off, the machine wants the center of the tool at x0y0, so in essence it HAS to jump, doesnt it?

You apply comp with a move towards the job and remove comp with a move away from the job. Try not to apply/remove comp on a non move block.
Don't think of the centre of the tool, just the profile. Except for your start and finish points. For a 1" cutter you need to stand off 0.501" at least. A comp move of 0.001" is ok.

I feel sorry for you. Your guy at work sounds a real numpty. You're interested...you'll get there. Soon you will be showing him what to do. Keep asking.

[glenthemann]

For a 1" cutter you need to stand off 0.501" at least. A comp move of 0.001" is ok.

I feel sorry for you. Your guy at work sounds a real numpty

By stand off, you mean the move in which i apply comp has to be atleast the radius of the tool away from the part, before I actually move in on it? Im not sure I follow, I guess the word stand off is confusing me as you referred to that when non-comp programming (which I understand and makes perfect sense, you have to add the radius of the tool to any numbers)

What I am wondering is on a G0G41/G42 x,y axis move, does the comp get applied on that move, and how is it applied; would the tool jump over its comp value in the correct direction immidately and then move to the G0 location, or does it interpolate along with the movement? Or does the comp get applied on the move AFTER the G0G41x,y move?

Correct me if I am wrong, but there has to be some sort of movement to a position prior to initiating the G41/42 correct? Afaik comp calculates compensation base on the previous position and the next upcoming position for a point, so if I were to just go into mdi (or write a prog, but why?) and punch in G90G54;G0G41x0.0y0.0, in theory since there was no previous motion would the comp just go anywhere? or would it base it off of the last position being the reference point?

The guy at my work isnt so bad, he is more of a lathe man himself, I actually prefer the mills, but will be getting more into lathes as well (im just more comfortable with the mills at the moment), we have a swiss and a few other regular lathes, and are going to be getting a turning center). Hes been in cnc since it beginnings and along the way picked up some old habits that were once the norm I suppose, and CNC has advanced a lot since then, he doesnt do any parametrics, messes with subprograms a bit but thats about it.. I have pretty big ideas as far as parametric programming goes, im a mathy kinda person and as I said before ive been programming for a long time and that is more my real style and interest. Basically he knows what works and may not be able to explain it the best, but in his own words he says cutter comp is scary because you dont know where the machine could go and all machines apply cutter comp differently (please correct this if wrong).. and really I think its just a lack of true understanding of the concept and its "exceptions". But like I said, what he does know and understand suffices and makes damn good parts, I just know I can take it a step, or maybe 50 ahead. Mainly what he has over a lot of people and myself is experience; he knows a LOT about all sorts of tooling, what works and waht doesnt, he can tell you what kind of steel or aluminum a chip is by putting it in his mouth, speeds and feeds for various depths of cut and tooling all in his head that no book can ever tell you. He does use comp for some things, but he uses a 0 tool diameter and just changes it as the part wears, still programs his old way and I guess it eliminates any comp weirdness, but then again I guess kind of masks any comp errors that would most likely be catastrophic if using the real tool diameter and positions right from the drawing with no stand off.

Anyway, im enjoying going into this trade, I chose this over engineering haha, schools just not for me, I enjoy learning things on my own. That doesnt mean I wont be taking any courses, boss has already said we're getting gibbs and he wants me to fully master that stuff, so until then I am getting to master the basics, as I really do feel this is necessary before jumping intoany cadcam software

PS.

Can you see anything wrong with my previous code as to why the leadout move on the finish seems to move linear rather than on an arc? I guess its the G65 trickery playing a trick.. but im not sure. Oh and I can just do my comp lead ins fully above and away from the part to eliminate any crashing right? ie

G90G54G0x2y-1
G43H1Z5.0
G0G41D1 y0.0
G0Z-1
G1x-1.0
G0G40y-1

But with the Z move after the comp initation woudlnt the comp use that point to compensate? or would it ignore position movements that are not within the current plane? in this case would I have to specific a G17 - or I guess g17 is implied via paramater?

[ChattaMan]

Try and do your Z move before applying comp. A comp move takes the next block info for working out it's position. You're comping in X,Y not in Z.

G0 X0 Y0 (rapid to start position, no comp)
G1 Z-1 F100
G1 G41 D1 Y1 (asking machine to move to Y1 but take into consideration the radius of the tool, 0.500". So C/L of spindle is now at Y0.5 but the edge of the 1" cutter is at Y1.)
G1 X-5 F200
........

Make any sense.

Try my finish pass I posted earlier to see if it works.

Look at cutter comp in the manual, but it goes way overboard.

Comp isn't scary and you do know where the machine is going to go, unless you don't know how to use it!!

[glenthemann]

Try and do your Z move before applying comp. A comp move takes the next block info for working out it's position. You're comping in X,Y not in Z.

G0 X0 Y0 (rapid to start position, no comp)
G1 Z-1 F100
G1 G41 D1 Y1 (asking machine to move to Y1 but take into consideration the radius of the tool, 0.500". So C/L of spindle is now at Y0.5 but the edge of the 1" cutter is at Y1.)
G1 X-5 F200
........

Make any sense.

Try my finish pass I posted earlier to see if it works.

Look at cutter comp in the manual, but it goes way overboard.

Comp isn't scary and you do know where the machine is going to go, unless you don't know how to use it!!

Well sadly I cant try your previous as we finished the parts today, im moving onto a new program now.

So since it is comping in x and y, any z movement is okay, but should just try to avoid it?

New part im working on I have to mill 2 flats on a part that was turned, at the same height and then another flat that is lower, I plan on keeping the comp on the entire time, but I have to have a z movement when I move to the lower flat.

By the way, I was thinking of using a circluar interpolation at a high feed rate instead of using 3 g0 commands, guy at work said the machine may servo lag moving in an arc at such a speed and may not produce desired results.. I beleive him but I still want to try it out, any thoughts?

Also can you give any pointers for switching between g41 and g42?

Ive ordered myself the 'CNC Programmers Handbook' and it should be coming by the end of the week I hope, it should shed a lot of light on the more in depth questions I have that the manual doesnt answer (such as switching between g41/g42). Im hoping I can maybe get my boss to pay for half of it :haha: damn thing cost $100, but its a big book and should have tons of invaluable information that I want/need.

Thanks for the help!

[ChattaMan]

You are over complicating things. It's just logical and easy. Yes Z moves are ok but not immediately as you are applying the comp move.

rapid to position
down in Z
apply comp in X,Y move
then mill away happily in X,Y,Z.

It really is that easy. Just give the control a chance to see where its going.

I was thinking of using a circluar interpolation at a high feed rate instead of using 3 g0 commands,

No idea what this means!!. Don't try cutting the part in a G0 move. If you mean you are moving to the start of the next cut in a high feedrate arc, then that's ok if you are in fresh air. Doesn't matter if the arc isn't accurate, because of servo lag, because you're not cutting the part. But be careful if you are real close to the part, you might clip it. Don't run before you can walk.

Can't picture what your next part is from your description. Attach a photo from your mobile phone or something.

[glenthemann]

You are over complicating things. It's just logical and easy. Yes Z moves are ok but not immediately as you are applying the comp move.

rapid to position
down in Z
apply comp in X,Y move
then mill away happily in X,Y,Z.

It really is that easy. Just give the control a chance to see where its going.



No idea what this means!!. Don't try cutting the part in a G0 move. If you mean you are moving to the start of the next cut in a high feedrate arc, then that's ok if you are in fresh air. Doesn't matter if the arc isn't accurate, because of servo lag, because you're not cutting the part. But be careful if you are real close to the part, you might clip it. Don't run before you can walk.

Can't picture what your next part is from your description. Attach a photo from your mobile phone or something.

Here is the part, im not giving specific dimensions but the idea is that for time savings (although minimal), after the G1 facing the flat, instead of either having the G1 continue out until you can rapid to the other side without hitting the diameter of the part, or instead of G1ing until you just clear the part (.05"), rapiding forward, over to the other side and then rapiding back into position just before the other sides G1, you G1 to th e point where you would normally rapid forward, and instead perform circular interpolation at a high rate, keeping the identical distance around the part until it reaches the other side (ie, use a radius .05" bigger than the part for the arc, and it will center out there). It leaves out the dead time of G1ing to a single rapid position, and it avoids 3 lines of G0 commands and potentially be faster?

Its minimal time savings if it indeed does work, but we were worried that there might be some sort of servo lag in moving in an arc so fast causing not so much of an arc at all. Your right about the dont run before you can walk, but I havnt crashed anything yet.. messed up an er25 toolholder and collet and the other day I forgot g91 in my g28z0y0 and it just rapided strait down to the part, scared the **** out of me but no collision *phew*.

[HuFlungDung]

I've never run a Centurion, but the explanation of G65 sounds a little off. In actual operation, the machine must be in the correct start position before compensation is applied. There is no 'second position' for it to properly begin from, given the math of the program.

Maybe what the manual is talking about is that when using G65, the machine waits to apply compenation with the next commanded real movement. I used to run old Bandits that actually made some (dumb) attempt to move as soon as a G41/G42 was commanded, because the controller executed every line of code as it read it. But more modern controllers combine the compensating movement with the first real movement command. So maybe Centurion was attempting to do what modern controllers do, but there is still no forgiveness in their method for an incorrect start/end position. It has to be correct.

Usually when you see a machine make a linear movement where an arc was commanded, there is something wrong with the arc center coordinates, but the control just ignores those and moves to the arc endpoint.

[glenthemann]

I've never run a Centurion, but the explanation of G65 sounds a little off. In actual operation, the machine must be in the correct start position before compensation is applied. There is no 'second position' for it to properly begin from, given the math of the program.

Maybe what the manual is talking about is that when using G65, the machine waits to apply compenation with the next commanded real movement. I used to run old Bandits that actually made some (dumb) attempt to move as soon as a G41/G42 was commanded, because the controller executed every line of code as it read it. But more modern controllers combine the compensating movement with the first real movement command. So maybe Centurion was attempting to do what modern controllers do, but there is still no forgiveness in their method for an incorrect start/end position. It has to be correct.

Usually when you see a machine make a linear movement where an arc was commanded, there is something wrong with the arc center coordinates, but the control just ignores those and moves to the arc endpoint.

No I am certain the G65 works like I said. The way it is is you have a start position anywhere, turn on comp and then the G65x,y which acts as a ghost, or previous position, then you go to the pre-cutting position and the control calculates that position using the position specified in G65 as the last, and as normal the line next to the part.

For example, here is straight from the book. We're inside milling a 1x1x1 pocket

G0x-5.0y1.0
G41 D1 F10
G65 X0Y1 (no movement 'previous' comp point identical to point #4 of the part.)
G0x0.0y0.0 (in position
G1z-1.0
x1.0
y1.0
x0.0
y0.0
G65x1.0y0.0 (no movement, acts as the second point on the part at)
G40G0z0.0

which essentially means you can avoid start and finish position movements all together and just use G65 to put them in there without actually moving to those points. the exact control is a centurion 7.

The control calculates the center point, you are right and if it were too small it would give an error as it couldnt reach the points with such a radius, and if it was too large it would appear to be linear.. but it is not too large the number is identical to the radius used to lead in so I dont know. Im thinking my last G65 point was in error, but I dont have any time to really go back and check right now, maybe someday soon.

Thanks for the help everyone

[glenthemann]

got my prog running, runs in 16 seconds and I have the arcrapid feed up to 150ipm with no clipping or positional errors

I found out the parameter number for the rapid rate, but I cant seem to find out how to view that parameter.. oh well. 150 is fast enough. I actually set P1=150.0 and then used F[P1] in the program for the rapidarc feeds, makes it so i only have to change one line

I can tell guy at work isnt liking my methods

I was adjusting my diameter value for my 5/16 endmill and he saw that I had 0.3110 in there and was like "arg youre using full diameter values", he didnt like the P1 thing either haha

[ChattaMan]

Excellent, well done!
Your drawing made it clear what you were doing, a great help.
Can't fault your toolpath and I bet the cutter went where it was expected to go, without doing any "scary" jumps.
Yep, can see why your workmate isn't liking your methods. It's out of his comfort zone. Sounds like he's stuck in his ways and loathed to change.
The high feed arc to the opposite flat is a common method, well done as a newbie.

..."arg youre using full diameter values", ....Yeah and look, it works!

Wait 'till you're doing more complex profiles, writing and adjusting the sizes in half the time that he does it in.

You're best leaving out the G65 thingy, keep up the good work.

[glenthemann]

I actually had to make a change from my drawing once I got it running and ran through in single block with the height offset +1" higher (just to make sure it didnt rapid into the part or anything), and its a good thing I did. With the G90G54G0 on that side of the part, with the x value I had it would have come down on the part due to the left cut, so I had to start it off on the other side and all went well.

One thing I am wondering about, is the jumping, while there were no scary jumps, the tool does "jump" over when the comp is initialized, perhaps thats because my start point was so close? I mean, if I had started a few inches or more away then the jump woudlnt seem so obvious. I think that is what my guy at work is talking about.. im not sure, I dont think he really understands fully how the comp works, neither do I, I suppose, but I know I do at the moment a lot more than he does, Im just working out the bugs.

Here is how I start the program, I left my notes at work but I can use fake values again. Lets say the two smaller flats are 1" wide and .3125 from center (y0.3125 and y-0.3125)

I start the program off like this

G90G54G0x1.05y-0.312 (I gave the cutter 0.05" clearance)
G43H1Z0.05
G0G41x1.05y-0.3125
G0Z-0.1
G1....
etc

When the G41 is intialized, the cutter has to jump over in x by the radius of the cutter into position obviously, but is there a way so that I can get it so that the cutter stays in the same position as it was prior to initializing cutter comp? -This right here is why I dont think the guy at work likes cutter comp.

I was thinking of changing the original G90G54G0 value to be moved over in X by the radius of the cutter, but then that makes the previous point that the G41 uses to calculate non perpendicular to the surface, and thus the cutter woudlnt end up where I wanted it to start anyway. When I make the bigger arc to the longer flat, I calculated out the points and used my coordinate geometry math (good ol x^2+y^2=r^2) to find a radius such that the arc becomes perpendicular once it meets the line the flat is on. I gave myself +0.50 again for the edge of the flat, but I realized that the face that actually does the cutting ends up being .2" away from the face, I originally though the cutter would be positioned right on the edge of the point, and not from the x and y of the cutter.. sorry if thats hard to understand, I can make a drawing later perhaps, but its just something I realized about using comp.

All in all part runs good, got the cycle time down to 15 seconds and the arc feeds are well above 200ipm now. I found out the rapid rate is 1600ipm!!! I made a booboo . and had the wrong H value in there on my initial run and even with rapid on 10&#37; the cutter went bam into the part and I had to remake the jig ><

Learnin somethin new everyday and my boss asked me to show him the receipt for the book I ordered, so it looks like hell be paying for it

[ChattaMan]

No no no no no!!!

------------------------------------
"G90G54G0x1.05 y-0.312 (I gave the cutter 0.05" clearance)
G43H1Z0.05
G0G41x1.05y-0.3125
G0Z-0.1
G1....
etc"
-----------------------------------

your start pos should be y-0.812 (=y-0.312 and rad of cutter+ clearance)

G90G54G0x1.05 y-0.812 (I gave the cutter 0.05" clearance)
G43H1Z0.05
G0Z-0.1
G1G41D1x1.05y-0.3125(moves up to face applying comp!!)
G1X-1.05....
etc

You had a start pos the same as your first move (y-0.312)
You MUST stand away from the job, then move onto it while applying comp. Sheeesh!!
Just to start with, while you're learning, make your approach move at
90° to the face you are cutting....as in your drawing.
You put the C/L of your cutter on where the edge of the cutter needs to be. It jumps because when you applied comp it's putting the edge of the cutter in the correct place.

[glenthemann]

No no no no no!!!

------------------------------------
"G90G54G0x1.05 y-0.312 (I gave the cutter 0.05" clearance)
G43H1Z0.05
G0G41x1.05y-0.3125
G0Z-0.1
G1....
etc"
-----------------------------------

your start pos should be y-0.812 (=y-0.312 and rad of cutter+ clearance)

G90G54G0x1.05 y-0.812 (I gave the cutter 0.05" clearance)
G43H1Z0.05
G0Z-0.1
G1G41D1x1.05y-0.3125(moves up to face applying comp!!)
G1X-1.05....
etc

You had a start pos the same as your first move (y-0.312)
You MUST stand away from the job, then move onto it while applying comp. Sheeesh!!
Just to start with, while you're learning, make your approach move at
90&#176; to the face you are cutting....as in your drawing.
You put the C/L of your cutter on where the edge of the cutter needs to be. It jumps because when you applied comp it's putting the edge of the cutter in the correct place.

but starting from there with that x value put the tool onto the part, aka it would have rapided into it, so I guess I thought the wrong way around (lol) and put it on the other side so that the tool came around the outside rather than from the inside.

I guess I dont quite follow you about putting the centerline of the cutter on where I want it to be. What I mean is that if the start poistion and the comp position are the same in the X, then when the tool applies comp its going to move over the radius of the tool in the Xdirection to one side or another, but still be continuing forward in the y. Hence the jump I speak of.

[HuFlungDung]

I think you're confusing yourself by not following some simple rules, that may or may not affect what you see the controller doing. Not all controllers handle compensation the same way, or even correctly in all situations, so it is best to spell it out with correct syntax.

The rules:
1. No Z movements during a compensated path. Turn compensation on when the tool is at depth, turn it off (G40) before retracting in Z.
2. No rapid motions during a compensated path. Some controls will cancel compensation when G00 is invoked. Whether it turns back on in the next G01 move is arguable, because the path would require yet another lead in line to apply comp to the new profile.
3. The lead in to the profile is absolutely necessary. You cannot start with the tool on the profile. Do not envision the lead in position as a random point. It is the beginning of the path so far as the controller is concerned because it is from the lead in that the controller figures out which side of the path it must compensate to. The tool center begins on the lead in position, but the tool becomes tangent to the path by the end of the lead in movement. There is no jump unless you called compensation too early, which could conceivably cause the tool to be on the wrong side of the lead in. See rule 1.

[glenthemann]

I think you're confusing yourself by not following some simple rules, that may or may not affect what you see the controller doing. Not all controllers handle compensation the same way, or even correctly in all situations, so it is best to spell it out with correct syntax.

The rules:
1. No Z movements during a compensated path. Turn compensation on when the tool is at depth, turn it off (G40) before retracting in Z.
2. No rapid motions during a compensated path. Some controls will cancel compensation when G00 is invoked. Whether it turns back on in the next G01 move is arguable, because the path would require yet another lead in line to apply comp to the new profile.
3. The lead in to the profile is absolutely necessary. You cannot start with the tool on the profile. Do not envision the lead in position as a random point. It is the beginning of the path so far as the controller is concerned because it is from the lead in that the controller figures out which side of the path it must compensate to. The tool center begins on the lead in position, but the tool becomes tangent to the path by the end of the lead in movement. There is no jump unless you called compensation too early, which could conceivably cause the tool to be on the wrong side of the lead in. See rule 1.

Well I kind of have to have a z movement in the program.. makes no sense to turn it off, move over, down, turn it on.. would have to have another proper lead in and all. with the current part im making it is in a collet fixture and the bottom side I have to mill is in a pocket milled out for the cutter to fit in, I have to feed z down to that, and then up while in comp, I dont really have any other choice.

But thanks for the pointers