[swiss89]

I'm using cutter comp for a full radius groove, and no matter what I have tried, I end up getting a cutter comp alarm, or a tool path that I know is wrong from watching the machine coordinates. Any help would be appreciated. I am using a .100" full radius insert and using tool nose #8 for my comp # , and putting .050 in the geometry radius column. Here is my code, and attached is the profile that I would like to create. Thanks!

T0505(.100 FR GROOVE)
G96S200M3
G0X1.7
Z.350
G41X1.2
G1X.938F.003
G2X.878Z.380I-.030K0
G3X.630Z.500I-.120K0
G1X1.6F.050
G40G0X1.7
Z.650
G1G42X.938F.003
G3X.878Z.620I-.030K0
G2X.630Z.500I0K-.100
G1X1.700F.050

[oldgoat]

Check your geometry first. I do not recall what the error limit maximum is (usually parameter??), but your numbers do not add up.

.630 minor groove diameter + .120 radius = .870 diameter + .03 radius = .93 major dia. You seem to be missing .008 of diameter somewhere.....

[beege]

I'd be using a 9 for my comp number, driving off the center of the radius, not the edge.

[angelw]

T0505(.100 FR GROOVE)
G96S200M3
G0X1.7
Z.350
G41X1.2
G1X.938F.003
G2X.878Z.380I-.030K0
G3X.630Z.500I-.120K0
G1X1.6F.050
G40G0X1.7
Z.650
G1G42X.938F.003
G3X.878Z.620I-.030K0
G2X.630Z.500I0K-.100
G1X1.700F.050

Given your diameters of 0.938 and 0.630, the X coordinate at points 2 and 4 will be X0.8764, not X0.870. Also, the I and K values for the 0.120 radius are wrong. Following are the correct coordinates based on the radii specified and diameters of 0.630 and 0.938

Regards,

Bill

G00 X1.7000 Z0.3501
G01 X0.9380
G02 X0.8764 Z0.3800 I-0.0300 K0.0000
G03 X0.6300 Z0.5000 I-0.0032 K0.1200
G01 X1.7000
G00 Z0.6499
G01 X0.9380
G03 X0.8764 Z0.6200 I-0.0300 K0.0000
G02 X0.6300 Z0.5000 I-0.0032 K-0.1200
G01 X1.7000

[mcode]

I think the proper way would be:

.938 - (.03 * 2) =.878
.630 + (.120 * 2) =.870
a remainder of .008

X.8764 will cut, but the .03 rad. will be cutting past one quadrant.
If you G1X.870 to the start of the .120 rad. the arcs will be a full quadrant.

G0X1.7
Z.350
G41X1.2
G1X.938F.003
G2X.878Z.380I-.030K0
G1X.87
G3X.630Z.500I0K.12
G1X1.6F.050
G40G0X1.7
Z.650
G1G42X.938F.003
G3X.878Z.620I-.030K0
G1X.87
G2X.630Z.500I0K-.12
G1X1.700F.050

not trying to step on you Bill, you have my up most Respect

Mark

[angelw]

I think the proper way would be:

.938 - (.03 * 2) =.878
.630 + (.120 * 2) =.870
a remainder of .008

X.8764 will cut, but the .03 rad. will be cutting past one quadrant.
If you G1X.870 to the start of the .120 rad. the arcs will be a full quadrant.

G0X1.7
Z.350
G41X1.2
G1X.938F.003
G2X.878Z.380I-.030K0
G1X.87
G3X.630Z.500I0K.12
G1X1.6F.050
G40G0X1.7
Z.650
G1G42X.938F.003
G3X.878Z.620I-.030K0
G1X.87
G2X.630Z.500I0K-.12
G1X1.700F.050

not trying to step on you Bill, you have my up most Respect

Mark

Hello Mark,
Yes, I concur with you. In theory, there would be an interference cut on the 0.030 radii, unless a radius insert with slight side clearance were used; the norm. However, this interference is only 0.00001". Although this is an available Least Programmable Increment, in the overwhelming cases a 0.0001" system is supplied, so its unlikely that any interference would occur, even if the sides of the insert were perfectly parallel. Normally a Full Radius Insert will have side clearance far in excess of 0.00001; accordingly the program would work quite successfully.

It comes down to interpretation. As the OP had no Linear move between the 0.030 radius and the 0.12 radius, I simply calculated the points based on the number of geometry elements indicated in the OP's code.

Unless there were Typos in the OP's listed code, the main reason for the Cutter Comp errors would be caused by the I and K address used for the 0.12 radius cuts shown below.

Regards,

Bill

G96S200M3
G0X1.7
Z.350
G41X1.2
G1X.938F.003
G2X.878Z.380I-.030K0
G3X.630Z.500I-.120K0
G1X1.6F.050
G40G0X1.7
Z.650
G1G42X.938F.003
G3X.878Z.620I-.030K0
G2X.630Z.500I0K-.100
G1X1.700F.050

[mcode]

I agree, thanks Bill

[swiss89]

Thank you guys for the help! I tried the code that Bill listed and it worked. At least that's the way it looked when I viewed it on the graph. I still haven't cut the material yet. I do have a question on how you got your coordinates for point 2 and 4? I take .938"-.030"*2 =.878" Instead you have listed .8764" I'm also not clear on the two I-.0032?

Beege,I'm curious as to why you would use comp #9? I plan to set the center of my full radius groove tool at z zero, and use comp #8 and the code that Bill listed. If I were to use comp #9 how should I set my tool?

This is the first time I programmed something like this, and I would just like to completely understand what I'm doing and why.

Thanks again.

[beege]

Comp #9 can compensate all around the tool, especially for a tool with greater than 180 degrees of arc. You'd set it so that the center of the cutting tool diameter is zero. For example, if your tool has a .125" diameter, touch the tool off as you would on X and Z, and subtract .0625 from the Z offset, and subtract .125 from the X offset. I haven't needed this very often at all, but a couple of tiems it was the only way to adjust a programmed profile without going back to the calculator and changing program lines.

[angelw]

Thank you guys for the help! I tried the code that Bill listed and it worked. At least that's the way it looked when I viewed it on the graph. I still haven't cut the material yet. I do have a question on how you got your coordinates for point 2 and 4? I take .938"-.030"*2 =.878" Instead you have listed .8764" I'm also not clear on the two I-.0032?

Beege,I'm curious as to why you would use comp #9? I plan to set the center of my full radius groove tool at z zero, and use comp #8 and the code that Bill listed. If I were to use comp #9 how should I set my tool?

This is the first time I programmed something like this, and I would just like to completely understand what I'm doing and why.

Thanks again.

The radial distance between the Root Diameter of 0.630 and the Major Diameter of 0.938 is 0.154 ( (0.938 - 0.630) / 2). If you add the two radii together, ie, 0.030 + 0.120, the answer is 0.150. Accordingly, the tangent point of the two arcs if each respective radius is tangent to the 0.630 and 0.938 diameters, won't be on the centre line of the two radii. To retain the same Major and Minor diameters, as well as the same radii, you would have to include a linear "X" move of 0.008 (diameter move), between the two radii, as suggested by Mark, to have the tool path start and finish on the centre lines of the respective radii.

Although on all other occasions I've agreed with Beege, he is a very knowledgeable person, I can't on this occasion regarding using Imaginary Tool Type "9". The Tool Type is used to pass to the control the way in which the tool has been set. For example you may have set your OD cutting Full Radius tool at the part of the insert corresponding to 3.0 o'clock (Z + Side) and 6.0 o'clock (X - Side) of the radius. In this case, you would specify an Imaginary Tool Type of "4". For an OD turning tool, you could specify any of the following Imaginary Tool Types, 0, 3, 4, 5, 7, 8, and 9. Imaginary Tool Types 0 and 9 are the same. Whichever Imaginary Tool Type that is specified, the actual tool must be set to correspond. If you have set your tool at 9.0 o'clock (Z) and 6.0 o'clock (X), as would be typical of a Right Hand Turning Tool, then the only Imaginary Tool Type that will work correctly is Type "3". Tool Radius Compensation works all round the radius of all Imaginary Tool Types, not just Type 0 and 9.

Regards,

Bill