Need Help With Cutter Comp

[Pmp Audio]

Hi Guys,

I'm trying to figure out types of cutter compensation and if they are enabled on the NC. I have a Kitamura Mycenter 1 with Fanuc OMC 6 controls. My first question is how would one know if the NC has cutter compensation active and if my post is right?

For the most part have the keeping offset list organized, for example if I'm using T1 I'll use offset number 1 for height then I'll use offset number 21 for cutter comp. The second is what type of cutter comp should I use to offset a cut to change an X or Y dimension? Let's say want to remove .003 from a circular interpolation diameter I would use reverse ware and enter -.003 in offset number 21?

Thanks in advance,
Eric

[dcoupar]

I usually turn on comp with a linear move at least as large as the amount in the offset. So, for example programming a 2" diameter circle with a 1/2" end mill (programmed for centerline of the tool) would look something like this:

G0 G91 G28 Z0
T01 M06
G90 X0 Y0 S2000 M03
G43 Z0.1 H01 M08
G01 Z-0.5 F20.
G41 X0.75 D21
G03 I-0.75
G40 X0
G00 Z0.1 M09
G91 G28 Z0 M19

[mzar]

Hi there,

U can check your cutter compensation is active or not by looking the active G function (G41 or G42) in the Jog Mode. If the codes is active that mean the cutter compensation is active.

During Execution, you can see the active functions by using Standard display mode.

For wear off, you should make sure the process of cutting. Is it to make Island or Pocket, then u automatically can put - or + sign forr offset.

[Pmp Audio]

Below is what I got for a post. So looks like it's in order, now will the cutter comp work only on the X moves or on both the X and Y? There are three types of cutter comp Control, Wear and Reverse Wear. Would one use control and offset either -.003 +.003 for example? So if I'm cutting a square and I want to remove .003 I would just set the contour to control and set the offset as -.003? Also say I'm cutting a circle and would like to make the circle lager by .003 I would set the circle tool path to control and set the offset to .003?

T3 M6
G0 G90 G54 X2.43 Y5.38 S1069 M3
G43 H3 Z.25
Z.1
G1 Z0. F6.42
G41 D23 X1.85
G3 X1.75 Y5.28 R.1
G1 Y1.85
G3 X1.85 Y1.75 R.1
G1 X5.8425
G3 X6.5 Y2.4047 R2.15
G1 Y4.7253
G3 X5.8425 Y5.38 R2.15
G1 G40 X2.43
Z.1
G0 Z.25
M5
G91 G28 Z0.
M30

[dcoupar]

Once you activate G41, the tool is offset left of the path (in both X and Y) by the value in the offset register you specified (in this case, #23).

I've never heard the terms "control" and "reverse wear" used in regards to cutter comp. Most newer Fanuc controls have GEOM and WEAR offsets for both Length and Diameter. If you're using offset #3 for length and #23 for diameter, then it sounds like you don't have GEOM and WEAR, only "offsets", which can be used for either length or radius.

If your CAM system outputs "cutter centerline", then you'll only need to enter the difference between the programmed tool diameter and the actual diameter. You can enter it as a + or - to adjust your dimensions.

If your CAM system is outputting "part profile" then you'll need to enter the tool radius in the offset for that tool. You can then adjust the offset amount + or - to change your part dimension.

[mzar]

From my experiences, programming is easiest if we set the actual tool radius on the tool offset table. Any wear or offset of the tool will be included at the wear coulomb. U can modified it easily. If u use CAM software, dont forget to put the actual tool diameter and tool compensation during setup.

[chucker]

below is a link where there is some explaination of reverse ware

http://www.cnczone.com/forums/archiv...p/t-11805.html

[sinha_nsit]

Originally Posted by dcoupar I usually turn on comp with a linear move at least as large as the amount in the offset. So, for example programming a 2" diameter circle with a 1/2" end mill (programmed for centerline of the tool) would look something like this: G0 G91 G28 Z0 T01 M06 G90 X0 Y0 S2000 M03 G43 Z0.1 H01 M08 G01 Z-0.5 F20. G41 X0.75 D21 G03 I-0.75 G40 X0 G00 Z0.1 M09 G91 G28 Z0 M19

The given program appears to be for 1.5" dia circle. With radius compensation, we program for the desired dimensions only, as if the cutter radius is zero.