Newbie to programming Haas...

[Snortch]

At work, the only person that knew how to program the Haas lathe got fired a couple of weeks ago, I was asked to see if I could figure it out. I'm a Mazak guy and all this G code stuff is pretty alien to me (haven't used it since college, 7 or so years ago). Luckily there is a training manual for me to use.

Here's a program I made today to face a part. It works fine, but for some reason, after the G72 roughing cycle is finished cutting at .01, it does it AGAIN at .01...cutting air. This is just adding cycle time, doing nothing. I'm sure it's a simple fix, but darn if I can figure out what to do. Here's the block of code:

(ROUGH FACE)
T404
G54 M31
G50 S1200
G96 S1000 M03
G00 X4.5 Z0.15 M08
G72 P101 Q102 U0.01 W0.01 D0.025 F0.016
N101 G00 Z0.
G01 X7.
N102 G01 Z0.1
G00 Z1. M09

Thanx in advance!!! I think I may like this Haas if I can just get more experience in programming and running it.

[-Chris-]

Why the Q102 link to ebay porn

[txcncman]

You put W.01, telling you wanted to leave .01 on the face for a finish cycle to be done at a later time. And end block should be on the X7. line.

[Geof]

......Here's a program I made today to face a part. It works fine, but for some reason, after the G72 roughing cycle is finished cutting at .01, it does it AGAIN at .01...cutting air. This is just adding cycle time, doing nothing. I'm sure it's a simple fix,...

I think you are stuck with it.

I have been programming Haas lathes for more than 12 years and I have observed the 'redundant' pass at the end of a G71 or G72 cycle on all of them.

But in some circumstances, it is not really redundant if you are only using G71 or G72 and are not following it with the G70 finishing pass. It is equivalent to a spring pass to do a final clean up to remove any inaccuracy from tool deflection. Depending on the total amount being removed and the D and F values the pass at Z0.01 could be removing almost a full D value and if you have D 0.1 with a high feed rate there could be noticeable deflection. Then the final pass will remove a bit more material.

Depending on the material, accuracy and surface finish required you can juggle the D, F, U and W values to get the required accuracy and finish in the shortest time. For best accuracy and finish use U and W to leave a finish allowance and set D and F large to do the roughing as quickly as possible and then run G70 at a slow feed. For less critical work leave U and W at 0, make F moderate and don't worry about the G70 cycle.

[Snortch]

Why the Q102 link to ebay porn

Uhh,,,what? I didn't make any links.

[Snortch]

You put W.01, telling you wanted to leave .01 on the face for a finish cycle to be done at a later time. And end block should be on the X7. line.

Yup...I have another tool todo the finish. The roughing tool makes an extra cut nothing pass.

[Snortch]

I haven't figured out the G70 yet...I just have another block with the other tool for the finish pass. The Shop Supervisor said to always use a different tool for finish. I'm cutting cast iron and it's tough on the inserts.

[Snortch]

Uhh,,,what? I didn't make any links.

I see that there...no idea where that came from, and I can't edit it out. Crap, do I have some kinda malware on my computer? Running malwarebytes now to see. If a moderator can fix that, I'd appreciate it!

[Snortch]

I think you are stuck with it.

I have been programming Haas lathes for more than 12 years and I have observed the 'redundant' pass at the end of a G71 or G72 cycle on all of them.

My shop supervisor asked my why it was doing that, now I know what to tell him. Thanx!!!

[Snortch]

Why the Q102 link to ebay porn

I found it...it's not on my computer, it's evidently a part of CNCZone's advertising links. It's called "Skimwords".

[Geof]

If you are cutting cast iron it is more or less essential that you use the G70 with a second tool. You just complete the G72/G71 cycle then do a tool change followed by the G70. Something like this:

T404
G54 M31
G50 S1200
G96 S1000 M03
G00 X4.5 Z0.15 M08
G72 P101 Q102 U0.01 W0.01 D0.025 F0.016
N101 G00 Z0.
N102 G01 X7. F0.005(This feed is used by the G70)
G00 Z1. M09
(G28 or move to tool change position)
T505
G50 S1200
G96 S1000 M03
G00 X4.5 Z0.15 M08
G70 P101 Q102
G00 Z1. M09

Incidentally if you are running cast iron why do you have D so small? Surely you could be doing the rough facing at something like D0.075 or even more to save time. You may have to back the feed down to F0.01 but it would still be faster.

[txcncman]

Try making starting Z not evenly divisible by the D. You have starting Z of .15 and D of .025. Try D of .026 and see what happens.