Fanuc Deep Drilling Cycle Help

Fanuc 21i-T

I need to drill a 1" deep hole in grade 2 Titanium Bar Stock (CNC Lathe)
Using a .25 Cobalt Parabolic drill
Using fusion 360 to output my G-Code

M1
T0404
G54 (delete or I get Alarm)
G98 (Change to G99 or it sits)
G97 S1200 M3
G0 X0. Z0.615 (Z0.05)
G17 (Delete or I get Alarm)
G0 Z0.215 (Delete Wasted Move)
Z0.615 (Delete Wasted Move)
Z0.215 (Delete Wasted Move))
G74 X0. Z-0.1 R-0.05 Q0.05 F0.003 (R0. or it moves in the X axis and snaps a bit after the drilling cycle before retracting)(Q0500 or I get Invalid Decimal)
G80
Z1.5
G28 UO. W0.

So A couple Things.

1. I don't like how that is outputted, so I hand edit every time. Would prefer not to. In parenthesis is what I change the code to do.

2. I don't get a full retract and the chips build up especially with Ti and it smokes my drill bit. I believe this Fanuc 21i-T will accept a G83 Deep Drilling Cycle with a full retract.

Any help or tips would be appreciated.

1) What are you using for a drill cycle in the CAM? All your wasted moves are your height definitions as best I can tell.

2) Most of this is going to rely on your post processor which has to be edited (like the Q0.05 output), and without seeing the CAM file it's hard to tell you what's going on.

If you want I would be willing to take a look if you want to invite me to the project or email me an exported .F3D file. I highly recommend the Fusion 360 CAM forum as well: Computer Aided Machining (CAM) - Autodesk Community

Atomkinder said:

1) What are you using for a drill cycle in the CAM? All your wasted moves are your height definitions as best I can tell.

2) Most of this is going to rely on your post processor which has to be edited (like the Q0.05 output), and without seeing the CAM file it's hard to tell you what's going on.

If you want I would be willing to take a look if you want to invite me to the project or email me an exported .F3D file. I highly recommend the Fusion 360 CAM forum as well: Computer Aided Machining (CAM) - Autodesk Community

Click to expand...

PM sent your way

Atomkinder - Your PM Box is Full

riseandgrind said:

Atomkinder - Your PM Box is Full

Click to expand...

I saw. You can send messages via A360 too, or just email me. Unlimited storage there!

riseandgrind said:

Fanuc 21i-T

I need to drill a 1" deep hole in grade 2 Titanium Bar Stock (CNC Lathe)
Using a .25 Cobalt Parabolic drill
Using fusion 360 to output my G-Code

M1
T0404
G54 (delete or I get Alarm)
G98 (Change to G99 or it sits)
G97 S1200 M3
G0 X0. Z0.615 (Z0.05)
G17 (Delete or I get Alarm)
G0 Z0.215 (Delete Wasted Move)
Z0.615 (Delete Wasted Move)
Z0.215 (Delete Wasted Move))
G74 X0. Z-0.1 R-0.05 Q0.05 F0.003 (R0. or it moves in the X axis and snaps a bit after the drilling cycle before retracting)(Q0500 or I get Invalid Decimal)
G80
Z1.5
G28 UO. W0.

So A couple Things.

1. I don't like how that is outputted, so I hand edit every time. Would prefer not to. In parenthesis is what I change the code to do.

2. I don't get a full retract and the chips build up especially with Ti and it smokes my drill bit. I believe this Fanuc 21i-T will accept a G83 Deep Drilling Cycle with a full retract.

Any help or tips would be appreciated.

Click to expand...

Hello riseandgrind,
As Atomkinder points out, the output of your code is a Post Processor issue.

With regards to the G74 cycle, if you're not aware, this is a Face Grooving Cycle that doubles as a Face Peck Drill Cycle by ensuring that the "R" argument is specified as Zero. When used as a Face Grooving Cycle, R is to specify a Relief amount in X of the tool at the bottom of the Groove.

Has your machine got Live Tooling and a Y axis? Given that you get an alarm when G17 is executed, I'd assume that there is no Y axis. G17 is to select the X,Y plane. What is the alarm number that occurs when G17 is executed? With no Y axis, the MTB may have forced a default of G18 and that no Plane selection is required, or possible. The control may accept G18, but it may not be necessary to specify it.

G83 may not be available unless the machine has live tools.

Regards,

Bill

angelw said:

Hello riseandgrind,
As Atomkinder points out, the output of your code is a Post Processor issue.

With regards to the G74 cycle, if you're not aware, this is a Face Grooving Cycle that doubles as a Face Peck Drill Cycle by ensuring that the "R" argument is specified as Zero. When used as a Face Grooving Cycle, R is to specify a Relief amount in X of the tool at the bottom of the Groove.

Has your machine got Live Tooling and a Y axis? Given that you get an alarm when G17 is executed, I'd assume that there is no Y axis. G17 is to select the X,Y plane. What is the alarm number that occurs when G17 is executed? With no Y axis, the MTB may have forced a default of G18 and that no Plane selection is required, or possible. The control may accept G18, but it may not be necessary to specify it.

G83 may not be available unless the machine has live tools.

Regards,

Bill

Click to expand...

G17, off the top of my head, I think it said Invalid Plain. I just delete it. Yes G18 works and will not get an alarm.
No Y axis. This is a Gang Tool Lathe as well.

What drill cycle are people using for an operation like this? Or is it something I should just hand code to do exactly as I want it?

Thanks

So I'm taking a look but your T4 in CAM in all your parts is a VNGG331 tool. Which part is this in your project?

Atomkinder said:

So I'm taking a look but your T4 in CAM in all your parts is a VNGG331 tool. Which part is this in your project?

Click to expand...

Sent you a PM on the AutoDSK forum.

riseandgrind said:

G17, off the top of my head, I think it said Invalid Plain. I just delete it. Yes G18 works and will not get an alarm.
No Y axis. This is a Gang Tool Lathe as well.

What drill cycle are people using for an operation like this? Or is it something I should just hand code to do exactly as I want it?

Thanks

Click to expand...

Hello riseandgrind,
With a Lathe with no Y, or Live Tools, as stated in my previous Post, the G74 Cycle with R omitted (assumed Zero Value), or specified as Zero, can be used, but the Tool is not retracted from the hole to clear the swarf. The Post Processor could be edited to be able to call the G74 cycle as either a Face Grooving Cycle (with Tool Relief in X at the bottom of groove), or as a Peck Drill Cycle. I doubt that G83 will be available in your control.

You could create your own Peck Drill cycles using the User Macro application and have them called with the standard G codes such as G81, G82, G83 etc. Your CAM software would output the standard Call Blocks as per the standard Fanuc cycles. There would be the added advantage of being able to improve on the Standard Fanuc cycles, such as being able to vary the size of the peck, feed rate and anything else you may think important.

Regards,

Bill

angelw said:

Hello riseandgrind,
With a Lathe with no Y, or Live Tools, as stated in my previous Post, the G74 Cycle with R omitted (assumed Zero Value), or specified as Zero, can be used, but the Tool is not retracted from the hole to clear the swarf. The Post Processor could be edited to be able to call the G74 cycle as either a Face Grooving Cycle (with Tool Relief in X at the bottom of groove), or as a Peck Drill Cycle. I doubt that G83 will be available in your control.

You could create your own Peck Drill cycles using the User Macro application and have them called with the standard G codes such as G81, G82, G83 etc. Your CAM software would output the standard Call Blocks as per the standard Fanuc cycles. There would be the added advantage of being able to improve on the Standard Fanuc cycles, such as being able to vary the size of the peck, feed rate and anything else you may think important.

Regards,

Bill

Click to expand...

Thanks for the input, and just like that, information I don't know how to apply
Time to read about macros.

Also how can you tell if your Machine or Fanuc will use the G83? My Fanuc Manual it says Fanuc 21i-TA So I am assuming its version "A"

It goes over G83 in the manual, but it seems more relevant to Milling VS turning.

Seems strange, that something as simple as a peck drilling cycle with a retract that clears chips would be such a mind bender for a machine like this.

riseandgrind said:

Thanks for the input, and just like that, information I don't know how to apply
Time to read about macros.

Also how can you tell if your Machine or Fanuc will use the G83? My Fanuc Manual it says Fanuc 21i-TA So I am assuming its version "A"

It goes over G83 in the manual, but it seems more relevant to Milling VS turning.

Seems strange, that something as simple as a peck drilling cycle with a retract that clears chips would be such a mind bender for a machine like this.

Click to expand...

There is a way to check and see if the control supports G83, it is a secret handed down from Father to Son, sometimes the instructions are tattooed on the head behind the right ear, and sometimes they are written on a very thin water soluble parchment ( in case you need to flush it). But I have it, I stole it from some Turkish pirates in 1822. The instructions are......try it.

Robert

riseandgrind said:

Thanks for the input, and just like that, information I don't know how to apply
Time to read about macros.

Also how can you tell if your Machine or Fanuc will use the G83? My Fanuc Manual it says Fanuc 21i-TA So I am assuming its version "A"

It goes over G83 in the manual, but it seems more relevant to Milling VS turning.

Seems strange, that something as simple as a peck drilling cycle with a retract that clears chips would be such a mind bender for a machine like this.

Click to expand...

Hello riseandgrind,
Create a short program containing a G83 cycle and execute the program in Single Block Mode. If the cycle doesn't exist in the control a P/S 10 alarm will be raised. If no P/S 10 alarm, observe the movement of the Z axis slide to determine if the Cycle Works. If no P/S 10 alarm, I'd suspect that the cycle won't work with the Main Spindle (spindle other than Live Tool Spindle).

Regards,

Bill

angelw said:

Hello riseandgrind,
Create a short program containing a G83 cycle and execute the program in Single Block Mode. If the cycle doesn't exist in the control a P/S 10 alarm will be raised. If no P/S 10 alarm, observe the movement of the Z axis slide to determine if the Cycle Works. If no P/S 10 alarm, I'd suspect that the cycle won't work with the Main Spindle (spindle other than Live Tool Spindle).

Regards,

Bill

Click to expand...

I will head out to the lathe in the morning and experiment. If I am stuck using G74, I read there is a parameter I might be able to change that would allow for a larger Retract, as it currently operates under the High Speed Peck mode right now I believe.

I think my spindle speed is a little to fast at 1200 anyways. I think I will prob just drop that down to about 700 and Hand Code a peck cycle of my own. Drill in about .375 and retract to a Z.01 the back in another .375 and Retract back to Z.01 then finish it off on the third pass.

It's grade 2 titanium with a .25 drill, so in theory I won't be exceeding the 3 times the diameter rule. Ill keep my Feed at .001 or .002 and see what I get.

thanks for all the suggestions.

litlerob1 said:

There is a way to check and see if the control supports G83, it is a secret handed down from Father to Son, sometimes the instructions are tattooed on the head behind the right ear, and sometimes they are written on a very thin water soluble parchment ( in case you need to flush it). But I have it, I stole it from some Turkish pirates in 1822. The instructions are......try it.

Robert

Click to expand...

At least I made it through a few helpful post before the infamous PM reply

Thanks Bud!

riseandgrind said:

I will head out to the lathe in the morning and experiment. If I am stuck using G74, I read there is a parameter I might be able to change that would allow for a larger Retract, as it currently operates under the High Speed Peck mode right now I believe.

I think my spindle speed is a little to fast at 1200 anyways. I think I will prob just drop that down to about 700 and Hand Code a peck cycle of my own. Drill in about .375 and retract to a Z.01 the back in another .375 and Retract back to Z.01 then finish it off on the third pass.

It's grade 2 titanium with a .25 drill, so in theory I won't be exceeding the 3 times the diameter rule. Ill keep my Feed at .001 or .002 and see what I get.

thanks for all the suggestions.

Click to expand...

Hello riseandgrind,
Following is a fairly simple example of a G83 cycle, if your control isn't equipped with the G83 cycle. In the example, the Macro is being called by Custom G code G83. This is achieved by registering the number 83 in any one, available parameter from parameter 6050 to 6059 inclusive. The Macro Program is then registered in a corresponding Program Number O9010 to O9019 inclusive. For example, if parameter 6050 is available and you use it, then the Macro Program will be registered under Program Number O9010.

I've not tested the program, but I can't see any obvious error. Take care if used.


Regards,

Bill


Call Block Example (Metric Example)

G83 Z-50.0 Q5.0 R1.0 E0.25 F0.25

Argument E(#8) is the Clearance when the Tool Rapids back to the cut zone after Retracting to the R Plane. If omitted, it will default to a value I've hard coded in the Macro Program (0.5mm in this example). This Metric Default will be converted to an Imperial value if G20 Mode is current.



Macro Program Example

O9010 (G83 USER MACRO)
IF[[#9 EQ #0]OR[#17 EQ #0]OR[#18 EQ #0]OR[#26 EQ #0]] GOTO100 (ERROR TRAP FOR OMITTED DATA)

#1 = 1 (SET DIVISOR FOR METRIC MODE)

IF [#8 NE #0] GOTO10
IF [#4006 EQ 20] TH #1 = 25.4 (SET DIVISOR FOR IMPERIAL MODE)
#8 = 0.5 / #1 (SET #8 TO DEFAULT CLEARANCE)

N10

#2 = #18 (MAKE WORKING COPY OF R - #18)

#3 = 0 (MAKE WORKING CLEARANCE VARIABLE - ZERO FOR 1ST LOOP)

WHILE [#2 GT #26] DO1
G00 Z[#2 + #3] (RAPID TO CLEARANCE)
#3 = ABS[#8] (SET WORKING COPY OF CLEARANCE)
#2 = #2 - [ABS[#17]]
IF [#2 LT #26] TH #2 = #26 (STOP OVER-CUT IN Z)
G01 Z#2 F#9
G00 Z#18 (RETRACT TO R PLANE)
END1
GOTO900
N100
#3001 = 1 (MISSING DATA - FIX)
N900
M99
%

riseandgrind said:

At least I made it through a few helpful post before the infamous PM reply

Thanks Bud!

Click to expand...

I'm sorry, I really wasn't trying to hurt your feelers. But really trying it is and always will be the best way to verify if a code is supported. I'm just keeping it funny.....Bud

litlerob1 said:

I'm sorry, I really wasn't trying to hurt your feelers. But really trying it is and always will be the best way to verify if a code is supported. I'm just keeping it funny.....Bud

Click to expand...

It's all good, I can take a ribbing, the amount of ass saving information I learn off this website is worth my humiliation at times LOL

UPDATE -

Just now had a chance to mess around with the mysterious G83 on my Lathe

Results - It supports a G83 Canned Cycle - Now I need to read up what does what inside the Canned Cycle so I can get this to work a little better then the G74 Cycle (High Speed Peck Drill) is how it operates at the moment.

You may like to read my eBook on live tool drilling cycles:
CNC Programming Skills: Live Tool Drilling Cycles on a Fanuc Lathe, S. K. Sinha, eBook - Amazon.com
You may pm me your mail ID for its free pdf.