Tapping cycle with a G94

[Lazarusman]

Need help. I programmed a drill tapping cycle, and it put in a G94. Connect me if I'm wrong, but cnc machines are preset to in/min. I got an alarm after attempting to run the program. It stopped on the G94 line. Kinda confused. 

[nickbe10]

5 minutes ago, Lazarusman said:

Need help.

Need more information

What machine ?

Rigid or non rigid tapping ?

Post ?

7 minutes ago, Lazarusman said:

Connect me if I'm wrong, but cnc machines are preset to in/min.

Feed rate format is not preset. Usually it is initiated on the safety line at the top of the program. At least in my post. This is because I use units / rev on rigid tap so I need to reset for safety before starting a new prog. If there is a rigid tap as the first tool it spits out a G95 at the toolchange and then G94 on the next toolchange, unless its another rigid tap.

So there are all sorts of ways this can be set up. You appear to have a disconnect between method and post. The resolution also depends on the machine manufacturer and model.

[Lazarusman]

It's a 7 year old Akira-Seiki Performa Jr.

I'm still new to programming, and I've only been machining for 2 years. When I post processed my program, the tap cycles don't act like tap cycles. They act like drills. I'm confused.

[guyw001]

I'm not sure about your machine control but if it's not tapping then you will likely also need an M29 in the program to initiate rigid tapping:

G95 (inch/rev)
M29 S415
G98 G84 Z-.32 R.1 F.0313
X1.4075

This is for a #6-32 tap so feed in inch/rev is .0313

[Lazarusman]

My machines use a Mitsubishi controller, which is non FANUC, and I'm not super familiar with its functions. As I have stated, I'm still relatively new to machining, and programming. I didn't know there was more than one tapping method used in CNC machines. I'm completely unfamiliar with lathes. (Haven't had those classes in my trade school, yet) I programmed the tap cycle, and Mastercam threw in a G20, and two G94s, per tap cycle. Also, I'm using a demo version of Mastercam, and one of my instructors told me that the problem is most likely because the demo version of Mastercam doesn't have my machine specifications loaded into it.

Thanks for all your help.

[jlw™]

Try G84.2 with F set to pitch in that Mits control.

[Lazarusman]

So. I have new information. Apparently my machines use a code I've never seen before. It's an E. followed by a number. I assume it has something to do with plunge rate, and retract rate as it applies to the tap cycle. Here is a sample.

 

N90 T8 M06
N95 G43 H8 Z1.5
N100 G00 G54 X-1.655 Y0. S220 M03
N105 G90 Z1.0
N110 M08
N115 G84 G98 Z-1.4149 R0.1 E16.0
N120 G80
N125 X1.655
N130 G84 G98 Z-1.4149 R0.1 E16.0
N135 G80
N140 G91 G28 Z0 M09
N145 G40 G49 G80
N150 M01
 

 

As you can see, there's no G94, but there's that strange E code.

What do ya'll think?

 

 

[crazy^millman]

3/8-16 TAP by Chance? E means TPI if that is the case would be my guess. If not 3/8-16 tapped hole what are you tapping? Why wasn't the post vetted before now? What has the company done before you started working with this?

[nickbe10]

57 minutes ago, Lazarusman said:

What do ya'll think?

I think it is an older Mitsubishi canned cycle. I ran an older Mitsubishi control for a while, the differences between them and Fanuc can be annoyingly difficult to determine.

I would try and get hold of a programming manual. It might not even be able to rigid tap.

The above code is typical for non rigid tap (aside from the E address). You could try replacing G94 with G95, although as Jay-dub pointed out usually there is some sort of spindle synching code (M29) but this is not always the case (Haas has no synch code).

You might have to use a tapping head. Is the spindle reversing at the bottom of Z feed? This should occur for any tap cycle.

[Lazarusman]

It's not recognizing it as a tapping cycle, so no, it isn't reversing at the bottom. (Raised Z 3 inches for dry run). They had been using a software called featureCAM... which sucks, but at least it'll tap. I compared the two programs, and the one that works, has no G94 or G95, it uses a G84 tapping cycle, with an E code. I assume the E code has something to do with feed rate in and out of the hole. I don't know how to calculate this variable, manually. Otherwise I'd just do it myself until I can get the full version of masterCAM.

Thanks again for your advice. 

[nickbe10]

12 minutes ago, Lazarusman said:

Thanks again for your advice. 

The E address, as Ron suggested, is probably the threads per inch. The control then uses this number to calculate an appropriate federate.

Note this is an option on Fanuc. You can either set up to use standard inches/min (G94) or as pitch which is inches /rev (G95). 

You will have to modify the post processer for either system to get this to work. Apparently this has been done on your Featurecam post.

For Mastercam you will need to initialize and format the E address variable. Extract its value from the operation and then output it via the tap postblock.

Probably not worth doing until you have the full version.