How to code this part.

[darinpeterson]

This might be more helpful, if someone has a minute. Can you show me how you might code this in general?

Also will you point out important parameters, like cutter radius offset and other things I should allow for?

Greatly appreciated...

Darin

Coding for a lathe please...

[M_D]

I'm not sure exactly what you are looking for. How I would go about programing and running the job would depend on many factors. One of a kind part? Small production run? Ongoing production? Is cycle time the main consideration, appearance, tolerance, all three, etc.

[sixsix]

How big is it and what's it made of.

What kind of lathe?

G-code, Mazatrol, offline?

What tooling do you have for the groove?

Barstock, collet or chucked?

[darinpeterson]

The difficulty were having is in coding the 180 degree arc on a Fanuc 6T. I don't care about figuring out much other than knowing whether there is G code that will cut a 180 degree arc, so feed rates and chuck speed are not a concern, nor are the actual part dimensions.

Say the groove starts at (X=-10, Z=-1), ends at (X=-10, Z=-2), and the cutter diameter is .5. If I could cut the groove in one pass, what would be the G02 or G03 code to do it?

Thanks,
Darin

[M_D]

I understand now what you are looking for, except I don't have enough time at the moment to do it, but I will check back later and if nobody has beat me to it will post code that should help you out.

[darinpeterson]

Originally Posted by M_D I understand now what you are looking for, except I don't have enough time at the moment to do it, but I will check back later and if nobody has beat me to it will post code that should help you out.

I thought it might just be a one-liner, but it sounds more complicated. I'll check back.

Thanks!
Darin

[M_D]

I guess since you are looking for code for a Fanuc 6T then this may not work (I haven't used that control), but I think it should. I suppose it is possible that control/lathe would requirements the radius devided into 1/4 quadrants or something, don't know though.

Example done in diameter programing, using a .125" full radius profiling cutter, measured to cutter radius center. The actual groove finish pass should only require one line, I included and approach where the same tool would cut the O.D. starting at the face to the end of groove radius.

The tool path is offset .125" (radius of cutter) from the part profile.

I hope this helps.

(G40 mode, no cutter comp, or if cutter comp is used only to dial in exact measurement)
N20 G01 Z0 X7.13
N30 Z-1.24 (corrected from Z-1.25)
N40 G03 X6.88 Z-1.365 R.125 (wraps around corner without actually cutting a radius)
N 50 G02 (X6.88) Z-2.135 R.385 (cuts actual groove)
N 60 G03 X7.13 Z-2.26 R.125 (wraps around corner without actually cutting a radius)


I added the tool path and tool positions to your original file and uploaded it to help visualize the tool path.

[darinpeterson]

Originally Posted by M_D (G40 mode, no cutter comp, or if cutter comp is used only to dial in exact measurement) N20 G01 Z0 X7.13 N30 Z-1.25 N40 G03 X6.88 Z-1.365 R.125 (wraps around corner without actually cutting a radius) N 50 G02 (X6.88) Z-2.135 R.385 (cuts actual groove) N 60 G03 X7.13 Z-2.26 R.125 (wraps around corner without actually cutting a radius)

The controller must be somewhat different. I can't use G02 and G03 with R. If I use G02 and G03, I have to use I and K. I can use R with G01. Have you written any G code for a 6T controller?

Thanks,
Darin

[M_D]

I have not used or written code for that control, so I may not be able to help you when it all said and done.

I have 1 machine where a radius (R x.xxxx) or chamfer (C x.xxxx) can be produced with a G01. In this case you would need (assuming your control will be the same in this regard) to divide the arc into 2 90º segments at Z-1.75.

This is what I would try, keeping in mind that I am not familiar with your controll or machine.

(.125" Full Radius cutter, tool radius offset figured into program)
N20 G01 Z0 X7.13
N30 Z-1.24 (corrected from Z-1.25)
N40 X6.88 Z-1.365 R.125
N45 X6.11 Z-1.75 R.385 (cuts 1st half of groove)
N50 X6.88 Z-2.135 R.385 (cuts 2nd half of groove)
N60 X7.13 Z-2.26 R.125

[M_D]

This might work using I and K.

Even though the previous code may not work on your machine, there was a typo I'll go back and edit with a note.

N20 G01 Z0 X7.13
N30 Z-1.24
N40 G03 X6.88 Z-1.365 I-0.125 K0.
N45 G02 X6.11 Z-1.75 I0 K-.385 (cuts 1st half of groove)
N50 X6.88 Z-2.135 I.385 K0 (cuts 2nd half of groove)
N60 G03 X7.13 Z-2.26 I0 K-.125

[HuFlungDung]

Darin,
I'm not sure why you specified working in X- for your example, but here are a few more permutations to try, as there has not been enough information given about this control's arc preferences:
(Maximum 180 degree arcs, incremental IK arc centers)
G01 X-10. Z0.
G01 Z-1.
G03 X-10. Z-1.25 I0.25 K0.
G02 X-10. Z-1.75 I0. K-0.25
G03 X-10.5 Z-2. I0. K-0.25
G01 Z-2.75

(max 90 degree arcs, incremental IK arc centers)
G01 X-10. Z-1.
G03 X-10. Z-1.25 I0.25 K0.
G02 X-9.5 Z-1.5 I0. K-0.25
G02 X-10. Z-1.75 I-0.25 K0.
G03 X-10.5 Z-2. I0. K-0.25
G01 Z-2.75

(max 90 degree arcs, absolute IK arc centers)
G01 X-10. Z-1.
G03 X-10. Z-1.25 I-5. K-1.
G02 X-9.5 Z-1.5 I-5. K-1.5
G02 X-10. Z-1.75 I-5. K-1.5
G03 X-10.5 Z-2. I-5. K-2.
G01 Z-2.75

(max 180 degree arcs, absolute IK arc centers)
G01 X-10. Z-1.
G03 X-10. Z-1.25 I-5. K-1.
G02 X-10. Z-1.75 I-5. K-1.5
G03 X-10.5 Z-2. I-5. K-2.
G01 Z-2.75

In a real world application, this type of path might only be suitable for a very light finishing cut, due to heavy side loading of the tool as it reaches bottom and tries to come up the radius wall. It would be better to make seperate roughing operations, beginning with a straight plunge to clear a groove almost to full depth in the center of the groove position, then rough each side, from the edge towards the center. But, maybe that is more than you wanted to know for now

[darinpeterson]

Hello,

Thanks for all of the replies!

I need to take some time to study the code that all of you sent. I appreciate your responses...

Darin