[jimmyjolly]

Hi all,

I have had a problem trying to work out tool wear compensation for our Turn Milling machines. When using an endmill to say finish off the diameter of a pocket on the face of a job, I use a G41 to apply tool radius compensation to the left and in G17 mode, how then do I apply a wear offset in the tool table?

I use a CAM system to program our machines (Multus and Macturn) and have been programming out the cutter wear until now, I need to get this resolved. I do not wan't to program full cutter compensation, just wear compensation so only small increments in the tool table.

I have tried (guessing) using the P (1-9) numbers in the tool table but can't figure out what direction I am meant to put the offset. It makes sense for turning but milling I am stumped, need a radius compensation rather than X,Y and Z offsets.

Anyone got any ideas?

Thanks, Jimmy

[deadlykitten]

hi

P(1-9) is for knifes; P9 is for a knife that works on the center of the radius, just like how it was an endmill; i don't know if P also affects milling

when i program milling on a mill i like to program tool center; thus, G41/G42 will reflect the difference between a new tool and a refreshed/regrinded tool, so will be 0 for a new tool

another practice is to program the part, thus G41/G42 will reflect the radius of the tool, so will be new_tool_radius for a new tool

on a lathe, i like to program tool center, and avoid G41/G42, but instead i edit the X offset value : smaller for a smaller pocket

[deadlykitten]

pls wait, another solution is on the way

[deadlykitten]

hello again, this is a 40x20 rectangle, cut in compensation :

 G137
 G17
 G00  X+20 Y+10 G42
 G101 X-20 Y+10  F...  G95
 G101 X-20 Y-10
 G101 X+20 Y-10
 G101 X+20 Y+15
 G40

some times special care should be taken when tool gets out of comp ( G40 ), because it comes with aditional movement; this sample blocks tool moving when leaving compensation :

 G00 Z=VSIOZ
 G00 Z=VSIOZ
 G00 Z=VSIOZ
 G40 G101 X=VSIOX/2*COS[VSIOC] Y=VSIOX/2*SIN[VSIOC]

thus, replace G40 with this; those G00 Z=VSIOZ are to delay the buffer, or else VSIO* will be read to soon

the final movement may be eliminated without VSIO*; please say if you need such a thing; kindly !

[ghyman]

Tell your CAM system the full diameter of the tool you are planning on using. (That is, the full diameter of a new tool.)

Make certain to have the CAM software output the positions of the center of the tool.
Without knowing the CAM system, I cannot give any further specifics as to the method to do this... but it sounds like you are already leaning that way.

For a Ø10mm endmill, the output for the above 40x20 rectangle will look something like this:
X0 Y0 (Approach move at CL)
G41 Y-5 (Move to bottom edge of part... Edge is at Y-10, minus 5 for the radius of the tool - dx from CL to cutting edge)
X15 (Left edge of part is at X20, again accounting for the 10mm radius)
Y5 (Y+10 - radius)
X15 (Right edge)
Y-5 (Back to bottom edge)
X0 (Back to center of part)
G40 Y0 (Clearance move)
(Extremely simplified output, but I think it serves to get the point across.)

Some shops call this "wear" or "partial" comp.
Your tool offset will be the difference between the radius of actual tool in the machine, and the target (perfect) tool.
This means that a reground tool that measures Ø9.5 will have an offset of 0.25 (0.5 diameter smaller than perfect, radius = 1/2 diameter)

The benefits of this approach are:
Small wear offset will not cause issues on the G41/G40 moves - Using actual cutter diameter means the machine has to have, in this example, an extra 5mm of movement on the G41/G40 lines, whereas using radius comp means the only extra movement needed is 0.25.
If the operator forgets and leaves the offset at zero, the resultant cut will at least be close to size.
The tool offset will be a small number, as it is only offsetting the tool by the wear amount.

Disadvantage:
This makes the program harder to read, as the tool radius is calculated into the cutter path.
If the shop is used to seeing full comp (where the measured diameter of the tool is used as the offset value) then changing to partial/wear can cause issues during setup and proveout.


I am pretty certain the Multus has a "D" in the offset column, that is where the value goes. We shipped out our last two Multuses (Multi?) about 2 weeks ago, so I can't walk out to verify that.

I am assuming you are talking about straight-up milling on a turning machine, and not the Okuma Mill-Turn feature, which allows you to use a turning tool in a live spindle and interpolate 1:1 with the spindle orientation to allow a turned finish on a milled part.

[deadlykitten]

my 1st example worked on tool offset, and the 2nd worked on radius; please see attached image for the input values for each example

2nd example is the right to do it, thus it reads "compensation radius" :
... if toolpath is on tool center, than input value is 0 for a new tool, or very small for a regrinded tool
... if toolpath is not on tool center, than input value is tool radius
... it works the same on G136 / 137 and 138

1st example may work or may not work; depends : this technique works fine as long as normal(=tangent+90 degress) at toolpath is intersecting the spindle center; also, there are particular cases when it may work, even if the normal is not intesecting the spindle center; thus, i recomend this technique for simple operations, but well, if the mechanism behind it is not understood, than it may deliver wrong simple operations for example, there is no problem if "spanner flats" are not straight, but on an arch, because part will still deliver it's functionality

crafting a part outside the dimensions specified by a technical drawing is something called "derogation" ? in this case, the part is accepted as functional

Disadvantage: This makes the program harder to read, as the tool radius is calculated into the cutter path

the "overheat" is not critical; is like a turning program that runs with or without compensation; so yes, the disadvantage exists, but it has no real impact on cutting/program overall duration

[deadlykitten]

hello, i have attached an image to show what happens when milling on lathe with CX, and applying corections from tool offset :
... yellow is a desired toolpath, designed on tool center : a straight line
... the upper point is the spindle center
... black lines represent the radius, thus X_axis / 2 when going with compensation = 0
... black circles represent a compensation_value
... if the compensation_value is input as a tool offset corection, than all black lines will get shorter with the compensation_value
... the blue dots represent the tool new positions, after aplying the corection from tool offset; result : a broken line

applying corections from tool offset delivers wrong toolpaths, but the final result may still be functional

if corections are aplied from tool radius, thus using G41/G42 and a compensation value <>0, results are correct, but if the tool holder is a bit offset, for example mines have default X=-40,Y0 while in reality it's center may be deviated, than :
... if G136 or G137 is used, than the final toolpath is wrong, even if the programing method is correct
... if G138 is used, the than final toolpath is geometrical correct, but is translated with holder deviations, or maybe i should say because of missalignments

however, since holders should come with an inspection sheet, proving their dimensions are correct, than all this deviations are at a scale that does not matter for most milling operations on lathe

[jimmyjolly]

Wow, thanks for the help guys.

Using Featurecam so and the program is outputting the centre of the cutter so I need to apply a wear offset only. I have leads in and out for the machine to apply the cutter comp so that shouldn't be a problem.

I am applying the G41 ( cuttercomp on left side) on the lead in as I would with say a normal milling program and the G40 command is the line after my lead out.

I guess the difficulty I am having is getting a definitive answer as to how to apply a wear offset on a milling tool in a Turn Milling machine in G17 mode or G119 mode ( not quite sure why it isn't G19 but that's Okuma)

We don't have a radius or diameter offset in the tool table for our Multus and Macturn (and from memory the LB3000's I have run didn't either) only nose radius compensation in X Z and Y plus a P direction.

On an Okuma mill no worries you have a diameter offset, but all the mill turns I have used no diameter offset function, just tool nose radius (which in my understanding is only used under a G18.

Here's my tool table :

Attachment 336468

Attachment 336470

If you could show me what offset you change in your tool table in say G17 mode or G119 mode , that would be a big help.

Thanks,

Jimmy

[deadlykitten]

so I need to apply a wear offset only

hy, is not "wear", but "correction", because you may need to do so, also on a new tool yes, i know, on the monitor, the label says "wear", but is just a translation; thus, consider a wrong translation, for a field, where you input the desired "corection" to deliver your shape

I have leads in and out

you may work like this, or start & end directly into a compensation position, thus without unnecesary movements

If you could show me ...

nose-r compensation declare them bought equal with the "correction" you need

and from memory the LB3000's I have run didn't either

i have such a machine, and the examples that i post were tested on it i have input "corrections" in "nose-r compensation"

On an Okuma mill no worries you have a diameter offset, but all the mill turns I have used no diameter offset function, just tool nose radius

this is because of the interface that may lead to wrong understanding; compensations works on radius, for bought mill and lathe, while on the mill interface is displayed "DA" and "R comp", thus if you see bought things you don't know if is diameter or radius

i have seen "R comp" just a few days ago, but i knew that "DA" works on radius

[OkumaWiz]

The Okuma is designed so that you put in the actual tool diameter when using comp. So for a .25 dia tool you would put in a .125 radius comp. The program will then want to be programmed from the edge and not the center. This gives you realistic part dimensions in your program. The wear register will then adjust for the wear from actual radius. If you are programming from the center, then you will need to get the optional negative comp option in order to accomplish what you want using only the wear register with a zero in the radius field. Your machine should take the larger of either the X or Z radius comp setting to use with the G41\G42.

Best regards

[jimmyjolly]

Ah ha so there is option I need then Okuma Wiz? Come to think of it I remember now doing a test in an LB3000 and the wear comp would work only in a positive direction. I will speak to Okuma Australia about the option. Thanks for your help!

[deadlykitten]

The Okuma is designed so that you put in the actual tool diameter when using comp

hello positive radius is only for lathes; ± works fine on mills > this is another "team vs team"

[jimmyjolly]

Have spoken to Okuma, it is a software upgrade with another option in built. We will have to work around it for now but thankyou for all the help!

[deadlykitten]

Have spoken to Okuma, it is a software upgrade with another option in built

hy for what is this upgrade ? to allow negative radius ?