[underthetire]

All you need is a simple float holder also know as a compression tap holder. No auto reversing head is required. If you found one that only had .5 or less in/ out float you'd be fine.

[bob1112]

Can you offer sample code for this operation? All my CAM programs will want to output G84 so I might need to adjust my post for this machine.

[underthetire]

I always just did a g1 in reverse and g1 out. In inch per rev mode. There may have been a float tap cycle, I don't remember. The extent of my programing now days is setting up lasers and ballbars for the most part.

[angelw]

So when we lock up feed/rev and feed in/out, will a simple axial float holder get it done or do you need some auto reverse head and all that?

Bob,
Yes, a simple axial (Compression/Extension) holder will work.

On blind holes, when tapping close to the bottom of the hole, and where the tapping depth needs to be consistently controlled, a tap holder that has a freewheeling area is available. When consistency of depth is required with this type of holder, a dwell with G04 is programmed after the block containing the Z depth move, and before the spindle rotation is reversed. Most of these holders work via the process of the tap continuing to feed whilst the Z slide remains stationary due to the dwell.
1. The spindle of the holder extends until its drive pin inside the holder, finds an annular groove which allows the tap holder spindle to rotate freely with the machine spindle and workpiece.
2. When the spindle direction is reversed, the tap holder continues to rotate with the work until the drive pin engages in a drive slot on the Z minus side of the annular groove as the Z axis feeds in a plus direction away from the workpiece.

Are you further saying that if we cannot enable the macro options in the machine, you can otherwise upload macro routines within a part program?

No, the machine must have the User Macro executable available. It just may not have been supplied as an Option ordered by the customer. It may be available in the control for use by the MTB (for tool change Macro etc), but because the machine is basically being supplied without the Option, the User Macro inputs via the keypad are not supported. In this case you can write a Macro program via a PC. But if you control doesn't have a Macro variable page where values can be registered, then your control effectively does not have the option. In this case a Macro program will be rejected by the control, even though the syntax may have been correctly written using a PC.

Following is an example of coding the tapping process in the CNC program. Depending on the MTB, the spindle reverse may have to be programmed as in Example 2. Write a sample program and observe the operation with the program cycling in fresh air.

Use G32(G code system A), G33(G code system B) instead of G01 to inhibit Feed Rate and Spindle Speed Override.

(Metric Example 1)
T0101
G97 S600 M03
G00 X0.0 Z5.0
G32 Z-20.0 F1.5
Z5.0 M04
G28 U0.0 W0.0
M01

(Metric Example 2)
T0101
G97 S600 M03
G00 X0.0 Z5.0
G32 Z-20.0 F1.5
M04
Z5.0
G28 U0.0 W0.0
M01

Regards,

Bill

[bob1112]

Bob,


No, the machine must have the User Macro executable available. It just may not have been supplied as an Option ordered by the customer. It may be available in the control for use by the MTB (for tool change Macro etc), but because the machine is basically being supplied without the Option, the User Macro inputs via the keypad are not supported. In this case you can write a Macro program via a PC. But if you control doesn't have a Macro variable page where values can be registered, then your control effectively does not have the option. In this case a Macro program will be rejected by the control, even though the syntax may have been correctly written using a PC.


Bill

Maybe you can clarify a bit the use of the PC for this. Are you saying that you STILL need macros enabled to load a macro via PC? How would you go about doing that? Maybe a sample macro? I assume these would not go to part memory so maybe there is a special character for the control to recognize a macro like a # sign in front of the macro variable? Just not understanding how to load via PC.

I will have to see if this is a bit change for the macro option. I certainly want to learn more on this subject.

[angelw]

Maybe you can clarify a bit the use of the PC for this. Are you saying that you STILL need macros enabled to load a macro via PC? How would you go about doing that? Maybe a sample macro? I assume these would not go to part memory so maybe there is a special character for the control to recognize a macro like a # sign in front of the macro variable? Just not understanding how to load via PC.

I will have to see if this is a bit change for the macro option. I certainly want to learn more on this subject.

Hi Bob,
Maybe you can clarify a bit the use of the PC for this. Are you saying that you STILL need macros enabled to load a macro via PC?
You can load a program that contains Macro Statements, but the control will error when you try and run the program. You upload the program containing Macro Statements in the same way a conventional CNC program is uploaded. Your could write something like the following, upload it to the control and try to run the program. If the option is not available, the control will raise an alarm; no harm done.

%
O1000
#1=1
M00
M30
%

On early Series 0 controls, very few had User Macro B, many had Macro A, and equally many did not have that option at all. With either version, there will be a Macro Variable Page available. If your control does not have this page, then the options does not exist with the control.

The fact that your control has a Macro Button that launches a blank page, MAY indicate that the feature could be turned on via an Option parameter, but mostly it was additional software that had to be added.

Regards,

Bill

[daborcito]

Hi Guys, I have a problem with the codes G83 and G84 on my fanuc OT control
the machine is a Nakamura lathe and I tried different thinks typing the lines
and allways gave me error message #10 (an Unusuable code was commanded)
I did for G83:
T0606
G00X0.0Z20.0
G97S800M03
G83R1Q4Z-36.0F0.08
G00Z20.0
G28U0W0

and for G84:
G00 X0.0 Z10.0
G84 Z-33.0 R8.0 F1.125
G00 Z10
any help please?
thanks guys!

[angelw]

Hi Guys, I have a problem with the codes G83 and G84 on my fanuc OT control
the machine is a Nakamura lathe and I tried different thinks typing the lines
and allways gave me error message #10 (an Unusuable code was commanded)
I did for G83:
T0606
G00X0.0Z20.0
G97S800M03
G83R1Q4Z-36.0F0.08
G00Z20.0
G28U0W0

and for G84:
G00 X0.0 Z10.0
G84 Z-33.0 R8.0 F1.125
G00 Z10
any help please?
thanks guys!

Unless the machine has Live Tooling, then its unlikely that your control has the G83 and G84 canned cycles and the P/S10 alarm point to these cycles not being available.. If the machine is a conventional turning centre G74 is used as an End Face Drilling Cycle. This cycle is also used as a Face Grooving Cycle. The format for drilling is as follow:
G74 R100
G74 Z-25.0 Q5.0

Where:
R = Return amount between pecks
Z = Z depth target
Q = Peck amount

For tapping, the code is written long hand, or, if the control has the User Macro B option, a Custom Macro Cycle could be written. The two methods follow:



Long Hand Code to tap 1.5mm lead thread.
G97 S300 M03
G00 X0.0 Z5.00
G32 Z-20.0 F1.5
Z5.0 M04
G28 U0.0 W0.0 M05
M01

Code to call Custom Cycle. In this case the number 84 would be registered in parameter 0220 so that Macro program O9010 is called with G84.

G97 S300 M03
G00 X0.0 Z5.00
G84 Z-20.0 F1.5
Z5.0 M04


Custom Macro
%
O9010
IF [#26 EQ #0] OR [#9 EQ #0]GOTO100
#1=#5022
G32 Z#26 F#9
Z#1 M04
GOTO101
N100
#3000=1 (MISSING ADDRESS DATA)
N101
M99
%

Regards,

Bill