Illegal pitch fixed cycle

[Da Mann]

What this message means? I am running M32 Mazak.I am using "feed=1/n_thds*speed" formula but as soon it cames out the first hole. I got an error message "Illegal pitch fixed cycle". Help!!!!!!!!!!

[DavidB]

Hi

Can you post the G-code.

 

Welcome

[Da Mann]

( POSTED ON: 10-01-06 AT 22:48 )

G17G20G40G80G90G94G98

G54

( TOOL 6, DIA = .19 )

( NO. 10-32 TAPRH )

G0G28G91Z0.

G0G28Y0.

T6M6T6

S650M3

G90X3.4978Y-5.505

G43H6Z.5M8

G95G99G84Z-.6R.5F.03

X4.5978F20.31

X7.31

X8.41

X9.41Y-3.905

X8.31

X5.5978

X4.4978

X3.4978Y-2.065

X4.5978

X7.31

X8.41

X9.41Y-.465

X8.31

X5.5978

X4.4978

G80

G94

M9

M5

G0G28G91Z0.

G0G28Y0.

M30

[Takashi Sato from Ai Solutions.]

G95G99G84Z-.6R.5F.03

X4.5978　(F20.31)

 

pitch(feed) is changed in second hole?

[DavidB]

MasterShaker is right the second position for the tapped hole has a changed feed rate.

 

The G84 tapping cycles stays modal until a G80 so it alarms when a different feed is programmed.

Take out the Feed on the second position and I'm sure you will be good to go.

 

If your machine can take a 3 decimal feed use it F.031 for 32 TPI.

 

Also is T6M6T6 correct?

T6 M6?

 

HTH

[Guest SAIPEM]

If you're setup for rigid tapping using G95(UPR Feed) then your Feedrate is off.

It should be carried out to a minimum of 4 places so you'll need to reformat the F address in the your post.

1/32 = 0.03125 or F0.0312

The difference of 0.00125 is enough to break a tap.

 

The second line in the canned cycle has a feedrate greater than 1 while using G95 UPR feed mode.

 

Tool Change needs to be T--T--M06 if you want to stage the next tool.

 

If you don't then the M06 has to be on a line following the tool call.

T--

M06

 

 

If you are using Mazatrol Tool Data and WEAR or REVERSE WEAR as the cutter comp type in Mastercam, then you need to lie in the Mazatrol Tool Data for the ACTUAL diameter of the tool and enter the smallest allowable value.

 

 

If you want the machine to run completely like a Fanuc control then you need to use the EIA offset data page for Tool Length and Diameter Comp.

 

You need to consult the Mazatrol Parameter manual for EIA related parameters.

 

Review F80,F84,F88,F89 in addition to the previous parameters listed.

[camgeneration]

I used to have this problem at the last place i worked, i don't know if it was the post or v9, although you can remove the line manually from the code, there was a way i got that fixed it from posting out the second feedrate. I can't totally remember though- Is you tool defenition setup with the pitch, ie are you just entering the pitch on the toolpath page, or are correctly setting up the tool first( with pitch, and with the drop down cycle set at tap)

klm

[Da Mann]

This is so weird. I am trying to find how and where that the post defined that F.03. Well I don't know where it is coming from. After I rechecked tapping operation just to be sure I don't have .03 any where and posted again, voila there is F.03. It makes no different if I change feed to 5000 in. Thank your guys for the sharp eyes.

[3rdstring]

The F.03 comes from the definition of the tap. The G95 specifies that you're feeding in IPR so 32 TPI = 1/32 feed per rev. Also note what Sapiem said about the feed, it should be .03125.

[Guest SAIPEM]

Edit your formatting in your post to use this for the F address.

 

# --------------------------------------------------------------------------

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

 

fs2 15 1l.4 1l.3 #Decimal, absolute, 4/3 place

 

 

# --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

 

fmt F 15 feed #Feedrate