Rigig Tapping Error

[Rick Miller]

Hello All,

 

I recently purchased a new HAAS ST20SSY lathe with live tooling.

 

I'm getting an error 329 m code not defined.

 

if anyone has had this same issue I would like to hear your fix. I've included the code MasterCam X9 is outputting.

 

Thanks,

 

 

%

O0000

(3_CYL_SLEEVE)

(DATE=DD-MM-YY - 06-04-16 TIME=HH:MM - 12:43)

(MCX FILE - C:\\3_CYL_SLEEVE_BACKSIDE 3-31-2016.MCX-9)

(NC FILE - C:\\ROTEC_3_CYL_SLEEVE.NC)

(MATERIAL - ALUMINUM INCH - 6061)

G20

(TOOL - 7 OFFSET - 7)

( 7/16-14 TAPRH)

T0707

M154

M49

M8

G97 P218 M133

G99

G17

G00 G54 X8. Z1. C0.

X1.5

G95 Z-.65 F15.57

C90.

C180.

C270.

G00 G80

X8. Z1. C0.

M9

M155

M135

G53 Y0.

G53 X0.

G53 Z0.

M30

%

 

[AMCNitro]

G159 APL Background Pickup/Part Return (Option) G160 APL Axis Command On (Option) G161 APL Axis Command Off (Option) G184 Reverse Tapping Canned Cycle (X, Z, W, R, F)(Setting 130) G187 Accuracy Control For High Speed Machining (E)(Setting 85 G195 Radial Tapping (X,F)(Live Tooling)(Option) G196 Radial Tapping Reverse (X,F)(Live Tooling)(Option) G200 Index On The Fly (X, Z, U, W, T)

 

 

Hopefully that helps

[Rick Miller]

I just got off the phone with HAAS and the M49 should be a G49. MasterCam post error. Now I'm getting exceeds max federate.

 

T0707

M154

G49

M8

G97 P218 M133

G99

G17

G00 G54 X8. Z1. C0.

X1.5 ************************** This line ?

G95 Z-.65 F15.57

C90.

C180.

C270.

G00 G80

X8. Z1. C0.

M9

M155

M135

G53 Y0.

G53 X0.

G53 Z0.

M30

%

[Eric@HorsepowerInc.]

The reason being your set up for feed per revolution, your feed rate is incorrect. Good thing for the error/max feed settings! Should be expressed.. Example 1/4-20....F.05

 

HTH

[Rick Miller]

Isn't 14/1= .071426" * 218" = 15.57"

Then G95 inches /rev

I guess 15.57" per rev would cram the tap right to -.650" instantly.

 

 

I will look at my parameters in the morning and see if I ca find my mistake.

 

Thanks

[Machineguy]

On a lathe the pitch is the feed rate.

[Eric@HorsepowerInc.]

https://diy.haascnc.com/g-codes-lathes

 

Maybe this will help you in understanding the basic g-code needed and correct definition of each.

[Rocketmachinist]

You need to swap to ipm. you need a g98 call out to make the tapping cycles work correctly. Right now it is trying to feed at 15.57 inches per revolution.

[Rick Miller]

This is what I've figured out.

 

%

O0000

(3_CYL_SLEEVE)

(DATE=DD-MM-YY - 06-04-16 TIME=HH:MM - 12:43)

(MCX FILE - C:\\_3_CYL_SLEEVE_BACKSIDE 3-31-2016.MCX-9)

(NC FILE - C:\\3_CYL_SLEEVE.NC)

(MATERIAL - ALUMINUM INCH - 6061)

G20

(TOOL - 7 OFFSET - 7)

( 7/16-14 TAPRH)

T0707

M154

M8

G97 P210 M133 

G98

G17

G00 G54 X8. Z1. C0.

X1.5

G95 Z-.65 F15. ( 210RPM * .0714"Pitch = 15.0IPM Feed rate )

C90.

C180.

C270.

G00 G80

X8. Z1. C0.

M9

M155

M135

G53 Y0.

G53 X0.

G53 Z0.

M30

%

[Mike@Lustre]

HAAS shows the G95 as a end facing live tool rigid tap , unless you are running a Live tool , this is the wrong command G code , as other have stated it should be a G99

[Rick Miller]

This is with live tooling on the face of the part.

[Rocketmachinist]

You probably need a retract plane.

[Mike@Lustre]

need a M14 prior to the G95 , also has to be run in G99 and a M15 at the end , the M14/M15 is the spindle clamp lock/unlock

[Rocketmachinist]

Sorry for everything I said. Apparently the rigid tapping is written totally different from the normal live tool stuff and the book does have it correct. Traditional thinking would say that if you are calling up the main spindle that you use M03. If you are calling up the live tool you use m133. The main spindle has an encoder and will tell the control about fpr and the live tool can't use that data so it would need fpm. But only on this cycle they mix and match what you need to get everything put together. I just tried it and it worked- in single block. When i try to run it as a full program is where it starts to have trouble.

[TiGuy]

Hello and thank you for this update. I did figure this out. When I'm back at work I will post the code. Unfortunately MasterCam X9 is posting the NC code incorrect along with the spindle direction being M134 as cw? It will be obvious when I post it.

[Rocketmachinist]

that would just be a swap with in the post.

 

this is what i found that works but my machine might have some problems. (old sl-20)

 

T0101

M154

C0.

S100

G00 C45. X.5

M14

G95 Z-.5 R1.0 F.035714

G80

 

It worked but some times when I was running it I am getting a A axis overload error. I am not even tapping anything for real. I wonder if there is an encoder that is messing up on my machine. Some times I can get it to work other times I can't

[Matthew Hajicek - Singularity]

Be aware that for face-oriented vs cross-oriented live tools you may need to reverse your M133 / M134, as some live-tool lathes use a gear to make the orientation change.

[TiGuy]

I looked at the post a little for M133 M133 and didn't see anything that was odious.

[Rocketmachinist]

I use haas SL 4x lathe. The one that comes preinstalled with later versions of mastercam is really close and just needed minor edits.

 

But I have realized something intersting on my machine.

 

If I do this (doesn't directly deal with tapping but hear me out)

 

T0505

G54;

M154;

G04 P1. (I put the dwells in there because sometimes it goes through the lines of code too fast and doesn't have time to finish what its doing before moving onto the next operation.)

G00 C0.

G04 P1.

M14

G04 P1.

M133 P500

Z2.0

X1.250

G01 Z-.5 F4.

 

I get an A-axis overload error. Which is funny because it is literally cutting nothing, it errors before the tool even comes close to the material.

But if I do this

 

T0505

G54;

M154;

G04 P1.

G00 C0.

G04 P1

M14

G04 P1.

M155

M133 P500

Z2.0

X1.250

G01 Z-.5 F4.

 

It runs fine. I noticed how much the Caxis spindle load was shooting up when I turned on the main spindle clamp. It would go from 2% up to 30% and stay there when I had the spindle clamp engaged. So I decided to use the clamp instead and see what happens. No errors. So I think the Caxis load and A axis loads are tied into each other and the way around it is to not preload the C axis with any additional forces it doesn't need.

 

I am going to try rigid tapping again with no C axis and see if that works.

[Machineguy]

How small a tap can you get away with in live tooling?

[Rocketmachinist]

I have never rigid tapped. Only dry ran the programs and got an error. I think it might be because of the spindle clamp thing. I didn't have any problems with the live tooling with a .5 inch endmill.

[crazy^millman]

I have on other machines done as small as 2-56 with form taps.