[rideredcr]

Hi Everyone! Happy 4th!!

I am looking for a little bit of help programming a simple G02 half circle. I have attached a drawing. The arc closes to the spindle is perfect. The arc furthest from the spindle is incorrect.
Here is the info:

HAAS TL-1
Tool = Grooving tool with a .0625" radius- see picture for better idea of what I'm trying to explain here
Tool tip 6 is selected in my tool offset screen

Code:

G96 S300 M03;
T1111 M08;
G00 X2.1 Z0.025;

G71 D0.025 F0.012 P10 Q50;

N10 G01 X2.0 Z0.0;
N20 Z-0.5;
N30 G02 X1.0 Z-1.0 R0.500; - This is the line of code that produces the incorrect arc :drowning:
N40 G02 X2.0 Z-1.5 R0.500 ; - This line of code produces the CORRECT arc
N50 G01 Z-2.0625;

G70 F0.006 P10 Q50;
G00 X3.0 Z3.0;
M30;


My brain completely explodes when I'm trying to use cutter comp G41 & G42. Mostly because I seem to pick the wrong one 100% of the time.
I attempted to plug G41 into this program with zero effect, so I tried G42..............the only effect it seem to have was when it performed the G70 finishing pass, the tool offset off of the part (never touching) as if it was an end mill and it was compensating like it would on a mill.

Anyways, I'm not the best programmer. I'm self taught and I'm sure I have a bunch of bad habits. If anyone has some words of advice, I'd be more than willing to listen.

Thanks!!!!!

[yardbird1969]

I'm surprised either side turned out to spec without using comp. I don't see finish allowances U & W in your canned cycle? Im not a HAAS guy but try these numbers. I'd use them to make your part on my Fanuc 0i-TD....

G1 X2. Z.0
G1 X2. Z-.5625
G1 X1.875 Z-5625
G2 X1. Z-1. R.4375
G2 X1.875 Z-1.4375 R.4375
G1 X2. Z-1.4375
G1 X2. Z-2.0625

No G41/G42 I figured the comp into the tool path for a .0625rad tool using tip 6

You probably have this matter sorted by now? If not give it a shot and see what happens.

Oh yeah!!! Run out in wide open air first just to make sure.

Good luck!! Hope you can make out the picture? I know it's not awfully good..

Brent

Attachment 326276

[rideredcr]

I'm stuck on the idea that the Haas controller automatically compensates/off sets your tool. In the tool off set screen it gives you the option to enter your tool radius. I just always figured the controller knew how to generate the correct tool path based on tool radius and tool tip #. Correct me if I am wrong.
I removed I, K, U & W because when I had them in the program initially, the arc furthest from the spindle was larger than the arc closest to the spindle by the amount I had specified in W.

Thanks Brent! I can see your picture clearly. I'll give your program a go. I was so fixated on making my program work, I didn't even think to just crunch a few simple numbers and compensate that way.

[rideredcr]

Taking a second look at your code Brent, I don't believe I need to compensate in X i.e. X1.875. I believe my part od will be 1.875 instead of 2.000 like I need it to be.

[rideredcr]

Disregard my last post. I see what the reason for X1.875 is now

[yardbird1969]

Like I say I'm not a HAAS guy. On my Fanuc the only way the control compensates for the radius of the is using comp G41/G42. Typically on parts such as yours I save me some headaches and figure it in the code and be done with it.

See what you come up with using that code and post back. If I can help I'd be more then happy to.

Good luck

Brent

[yardbird1969]

As to the finish allowances. Yes you will not be able shift the Z at all in the canned cycle or over cutting will occur opposite the shift by the finish allowance amount. In this case I would write 2 different tool paths. A rough canned cycle path cutting smaller radius above the one inch dimension. Then finish with a different tool path cutting everything to spec and correct size using the same tool.

G71 & G70 in my opinion isn't best suited for this situation but if the X finish allowance is enough there is a possibility you achieve total clean up on the finish pass using the exact same code. I'd just play with it and see what happens.

You could expand on my code a bit to put small radius on each side of the .5" radius at the 2." diameter as not to leave a bur.

Brent

[rideredcr]

This is what I came up with and it worked great:

Programmed T1111- Tool tip #6 w/ 0.001 radius---------actual tool radius is .0625

G96 S300 M03;
T1111 M08;
G00 X2.1 Z0.025;

G71 D0.025 F0.012 P10 Q70;

N10 G1 X2. Z.0
N20 G1 X2. Z-.5625
N30 G1 X1.875 Z-5625
N40 G2 X1.0275 Z-1.0 R.4375--------------- I had to use X1.0275 instead of X1.0 like I wanted because I would get an alarm message-non modal
N50 G2 X1.875 Z-1.4375 R.4375
N60 G1 X2. Z-1.4375
N70 G1 X2. Z-2.0625


G70 F0.006 P10 Q50;

G00 X2.0 Z0.100

G1 X2. Z.0
G1 X2. Z-.5625
G1 X1.875 Z-5625
G2 X1. Z-1. R.4375-----------This line cleaned up the radius nicely
G2 X1.875 Z-1.4375 R.4375
G1 X2. Z-1.4375
G1 X2. Z-2.0625
G00 X3.0 Z3.0;
M30;

[yardbird1969]

Good deal!! Glad everything worked out for you.

Brent

[chunkymonkey]

you can also use just 1 line of G2 to go across the entire radius. No need for tool point if not using G41/G42. Also, when using the G41/G42, keep in mind that G41 COMP LEFT is in regards to which side the Tool is on the Tool Path. I found that making small charts showing sample paths, G41/G42, and G2/G3 arcs has been helpful to darn near everyone i know when they get into the programming end of things. Good Luck

[sinha_nsit]

Because G41/G42 is not being used, it did not make any difference, but tip number 6 is not correct in external machining on a rear-type lathe with Fanuc control.

[yardbird1969]

I think he said it was a haas don't know what the tips are on them or fanuc. lol...

Brent

[sinha_nsit]

Yes. He said Haas. I thought it would be same as that on Fanuc. I was not sure, so I explicitly mentioned Fanuc.