[rusticr6]

we have 1 TM-2 that we just got and i have been running a Sl-40 for a good while and i am familiar with G42/G41 on the lathe. But on the mill we have not used cutter comp yet and i was looking for a formula to compensate my endmill radius when i go from a linear to an angle.

something like: Radius x tan(angle)

is there anything like that?

in my haas SL-40 lathe book there is a couple of pages that give you the compensation for 1/64 and 1/32 radius. they give 1-89 angles and the x and z amount to compensate for it. i have been trying to figure a formula that would match these but i cant get it spot on.

thanks

[CNCRim]

You don't have cad/cad?. Hint: add half(radius) of the endmill to the geometry you are doing then calculate from there.

[SeymourDumore]

Rustic

I'm either stupid or just really confused. If you're using G41/42 on the lathe, then why do you need to worry about the tool radius? As long as the control has the proper tip rad and direction, then you don't need to worry about anything other than making sure the ramp-on/off distance equals at least 1xRad? If you have the proper tip radius defined, then all your blocks should contain real part dimensions.
The formulas in the HAAS book refers to programming angles and radiuses without tool comp.
The same applies to milling as well. The ramp-on/off move must be at least 1/2xcutter diameter. In case of a 1/2" endmill it must be .2501 or more.

[rusticr6]

Sorry seymour, i wasnt clear on that. i was only saying that we use tool comp on the lathe, not on the mill.
i want to be able to figure out how much to move past the real part dimension at a specific angle in relation to my endmill radius.

Newtexas- we have auto cad and i can draw the part at scale, then i can see where my tool will be on the drawing. but i want to be able to figure all this myself. when you say add half the radius that is only partially right because you will need to move a distance further than that. it will be specific to to that angle.

am i making any sense?? i dont want to sound crazy.


kind of like if you want to put a radius at the beginning and the end of a taper on a lathe- i have a set of formulas that will let me get all the dimensions needed. i have tried to apply these formulas but i cant seem to get the right answer.

so lets say you have a linear that is 2.000 long and then it ramps up at a 15 deg. angle. we are using the side of the endmill, not the face.
you would have to move to the center of the endmill plus a certain amount that would be specific to your endmill radius and the angle.

[SORCHEROR]

rusticr6,if you have cad,than its simple,draw your part first,than offset all the part lines by half the cutter your using,now you have the exact path your cutter should follow,just analzye all the points on the new geometry and use those to program,at least until you get a cam program,this should work well on almost all your parts,asuming your only using lines,arcs etc.for me i cut surfaces and slpines too so i ahd to get cam package

[Jarwalcot]

Rusti,

See if this information helps you any...

[SeymourDumore]

"""
kind of like if you want to put a radius at the beginning and the end of a taper on a lathe- i have a set of formulas that will let me get all the dimensions needed. i have tried to apply these formulas but i cant seem to get the right answer.
"""

That's the part I don't get. If you're using tool nose comp ( G41/G42 ) on the lathe, then there is no formula, nor do you need one. You just program the radius tangent to the taper and done. All you need to worry about is to move off the part enough at the end of the path as to not cause overcut during ramp-off. No formula.

Ditto on the mill. If you have the radius drawn, then you program the linear-radius-linear moves, and then move the tool off the path by at least .0001 + 1/2 diameter.
Here is a quick example with a .01 radius on a 45deg angle:

G00 X-1. Y0. Z1.
G01 Z-0.5 F10.
G01 G41 X0. Y0.
G01 X0. Y0.9959
G02 X0.0029 Y1.0029 R0.01
G01 X0.9971 Y1.9971
G02 X1.0041 Y2. R0.01
G01 X2. Y2.
G01 G40 X2. Y3.


This is a cut for 3 lines having coords:
(0,0 : 0,1 ) (0,1 : 1,2) (1,2 - 2,2)
that are filleted by a .01 radius.
Ramp on is done @1" long from X-1., ramp off is also 1" long to Y3., in each case perpendicular to the previous path.

[Webderland]

E=mc²

[rusticr6]

seymour: i am not using G41/G42 on the mill.
you are most likely more advanced in programming than i am.

how would you program the 2" line then transition to 15 deg. angle with a 1/2" endmill. Without tool compensation. and still receive a 2.000" line.

thanks for the laugh, web

[wganders]

Rusticr6, if you are really interested in trying to figure out how to calculate your cutter pathes, versus plotting it in CAD, you may need to take a Trig class. Before I discovered CAD I would have to trig all my moves.

[SeymourDumore]

Ah Rustic. What you're trying to do is handcode mill programs with nothing but a calculator and a piece of paper.
I could ask why, but won't. I won't because there is no acceptable explanation I could imagine.
But if you must handcode, then:
Suggestion A: Use G41/G42 with full radius comp. This way the only thing need to be figured out is the ramp-on/off move, which is easy.

Suggestion B: If you're not using comp, then draw the part in CAD, offset the path by the cutter radius and then handcode the offsetted path.

I'd strongly recommend the former approach.

[gar]

070928-2000 EST USA

rustricr6:

Suppose you have a line segment from -4, 0 to 0, 0. This lies on the x axis from X=-4 to the origin. At the origin the line direction changes to -15 deg. The slope of the -15 deg line is TAN (-15 deg) = - 0.2679.

If your cutter is above the X-axis, then it starts at -4, 0.25 and moves to 0, 0.25. Now the cutter has to move to a point on a line perpendicular to the -15 deg line at a radial distance of 0.25 from the -15 deg line. This can be done as an arc or a straight line but such as to not cut into the apex of the two intersecting lines.

Using the straight line method you continue on the same X-path until you intersec the bisector of the 15 deg angle. This point is at X1 and Y1 where Y1 = 0.25, and X1 = 0.25 TAN (15/2) = 0.25 TAN (7.5) = 0.25 * 0.1317 = 0.0329. From here your path is at a negative slope of 0.2679. If you go a path length of 1 along the -15 deg line, then the end point of the cut is X = 1 COS (15) = 0.9659 and Y = SIN (15) = 0.2588. Next you have to calculate the center of the cutter which is at a point 0.25 on a perpendicular line to the -15 deg line from the end point of the cut. See if you can calculate this point, and see if I made any mistakes up to this point.

Do you really want to hand calculate the cutter path? For a learning and understanding experience it is good exercise. But, you should have a background in geometry, trig, college algebra, and maybe a little calculus.

.

[SeymourDumore]

Ok, if you don't want to use CAD then try your hand at MAD, as in Manually Aided Design, AKA algebra.

By definition a line is:

Y=aX+b

In Gar's example:
The first line is :
Y=0X+0 or more specifically:
Y=0

The second line is:
Y=tan15X+0 or more specifically:
Y=tan15X

Now, with a 1/2" cutter on the positive side of the path you need to elevate each lines by the cutter radius, in this case offset by .25.

so, the new lines will be:
1: Y=.25

2: Y=tan15X + (.25/cos15)

What you need to do in order to avoid overcut is to figure out where the 2 lines intersect.
Easy. The point is where line1=line2

so,

.25=tan15X + (.25/cos15)

solved for X:

X=(.25-(.25/cos15))/tan15 =-.0329

Therefore the 2 lines intersect at the X instance of -.0329.
SO in order not to overcut the path, you have to write the G-code as:

G01 X-2. Y.25
G01 X-.0329 Y.25
etc etc etc.

Easy as pie.....

For a computer....


Or a convict.....

[Geof]

And now that everyone has explained it throw it all away and learn how to use tool comp. Don't waste months and months like I did because I had the idea tool comp is complicated. On a mill it is trivial, on a lathe a bit more involved because you need to take into account the tool vector direction but in all cases it is a heck of a lot simpler than doing the tedious calculations for manual compensation in a hand written program.

Also when you do it by hand you are stuck with using that tool diameter; with tool comp you can change tool diameter and compensate for undersize or oversize tools.

[SeymourDumore]

And Amen to that brother


I cannot possibly imagine anyone even making a viable argument against using full cutter comp - lathe or mill - other than perhaps playing it safe with thick fingered operators putting in wayyyy off diameters. In that case wear-comp is maybe fine, but no fingercamming there either.
The control has the function to help you. Figure out how it works and then forget all other means of programming. Period.

[rusticr6]

gar, that is what i was looking for. i dont fully understand it, but when i have more time ill look at it more closely.

it may sound silly or strange, but i really want to understand how this works. i want to know how the computer is making these calculations. i really dont have time to take any math classes, but maybe ill buy a book and try to self learn. i basically am the lead programmer in my shop. all we have is 6 people who have had no official programming training. i was on nights for 9 years and i was taught the basics and learned a lot from the haas manual and trial and error.

i am not trying to turn back the clock on what computers have done for programming.

haas has that intuitive programming now. i think thats what its called. like quick code but better. say you wanna make an 8 hole pattern. all you do is put in the BC and the degree from the 1st hole and it writes the program for you. easy right? so if you are new to the whole cnc thing you dont have a clue as to what the hell is on the program. all you know is as long as you have the right tool and g54 or whatever, itll put that 8 whole pattern. great and wonderful. but for me, i wanna know how it came up with all that crap. i guess i dont want to be dumber than the machine.

i can see that all of you guys that has tried to help me are intelligent. guess what? you knew how to get the answer i was looking for. some could say i was lazy by asking, but i was in a bind. i knew that i wasnt gonna be able to figure out tool comp on the mill in a afternoon.

i promise to you i will learn tool comp. just not right this minute.

i appreciate all of your advice, i really do.

[gar]

070929-2123 EST USA

rusticr6:

You need at least a high school trig, beginning college algebra, and plane geometry books. Try your library. The Handbook of Mathematical Tables and Formulas by Burington can be handy. However, it may not be in print anymore.

The first few chapters in a college algebra book may be sufficient for your needs. It is very good that you want to know why.

Hand draw the lines I described, then use any round object, a penny for example, and observe what happens when you take different center paths. What I described in the previous post is an outside cut around the vertex.

Change to the other side of the lines, do an inside cut, and see what the constraints are. See if you can figure out how to calculate the cutter path.

A good understanding of plane geometry will help you understand machining problems. Example: if you cut a cone at different angles and locations you can generate each of the following curves --- circle, ellipse, parabola, and hyperbola. So if you program a circular path, and then change the scaling in the X-axis, but not the Y-axis, then you have produced an ellipse.

It appears that you truely want to learn. This is good, and in stark contrast to some that want a specific answer and do not want to know why. When the same general problem reoccurs they will be back for another answer where if they had learned why, then they might have solved their own problem.

There are too many problems that can not be effectively solved without knowing why.

You can donate a fish to a man and it will solve his immeadiate hunger. But you can teach a man to fish and he can solve his immeadiate and future hunger. This is why many poor people remain poor. They are fed by government giveway programs. This may be necessary for emergency conditions. But not for generations upon generations.

.

[SeymourDumore]

Rustic

As Gar has said, it is commendable that you're trying to figure these things out.
I do however want to say that knowing this won't really help you in your everyday job. I do believe - having 2 kids age 9 and 14 - that the current math and algebra curriculum is all but useless, so anytime someone wants to advance him/herself is a good thing.
At the same time I'd rather spend the initial time with figuring out how EAXCTLy the machine control works. Knowing how vectors coordinates are arrived at by the computer won't help becoming a better programmer. Knowing what the controller does with those vectors however does.
You can, for many many simple profiles, handcode an airtight program as fast as any conversational or CAM software can, as long as you know EXACTLY how cutter comp works within your controller.
Please, do yourself a favor and experiment with all kinds of possible scenarios of cutting paths. Try to code them and the backplot or cut it on the machine. See what works and see what does not. If you find what does not, try to make sense of it and do not under any circumstances glance over it and say, the heck with Comp, I'll just do it without until it's good.
One thing to remember here: EVERYTHING IS POSSIBLE!!! with comp. If it can be cut by centerline programming, it can be cut with cutter comp programming. It is very important, and my recommendation would be to ignore any and every statement to the contrary.

And since you brought up conversational and bolthole drilling, you don't need conversational. Just look at G70/71/72 in your mill's manual. These are the G-code equivalents to do the same.

[gar]

071002-0834 EST USA

Here is a simple problem for you to decide how to make the part.

A block of 6061.

The part is a 10 x 6 x 6 rectangular block with a flat surface entirely removing one corner. The plane of the cut intersects the three points
X9 Y0 Z4
X10 Y6 Z1
X6 Y5 Z4
The corner surface is to be very smooth.

.

[cspeegle]

Try this for a tool nose radius compensation calculation:

http://toolingandproduction.com/arch...99/499shpt.asp

It should help

COS