Drill retract with feedrate

[AMCNitro]

Is there a way, within MC, to program a peck cycle to retract at a feedrate instead of a rapid?  Im sure we've all run into situations where we wish the drill(or whatever we're drilling with) would have extra exposed to the coolant so it could clear chips.

[Guest]

Custom drill cycle or macro....

 

The G8x cycles don't have any option for this....

[balnh]

You can go into machine definition and set rapid to max feed rate. Then uncheck drill peck drill cycles to get longhand, I think.

[Colin Gilchrist]

If you still want to use a Canned Cycle to drill your holes, instead of having to resort to "long-hand" output, you could also just slow down the Rapid Rate of your machine.

 

This can be done easily by Programmable Data Entry. First, make sure you write down the "default" value of the parameter before you change it!

 

The Rapid Traverse Rate on most Fanuc controls is parameter #1420. This value is a two-word axis parameter (also known as a long integer). That means that the individual address (XYZABC) is set using a "P" number, and the "R" value that follows is an integer (some are signed, these are not!). Depending on the "increment" of the input, the "range" will differ.

 

You can use a Manual Entry toolpath to insert this code as G-Code, directly into your program:

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P1 R500
N1420 P2 R500
N1420 P3 R500
G11
(PARAMETER ENTRY MODE OFF)

In the above example, I'm setting X, Y, and Z rapid traverse rate to 50.0 Inches per minute.

 

We can do the same thing, and only set the Z axis instead, like so:

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P3 R500
G11
(PARAMETER ENTRY MODE OFF)

Then, after the drilling operation is complete, we can set it back to whatever the "default" value is, but remember that we first have to know what the original value was before starting!

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P3 R6000
G11
(PARAMETER ENTRY MODE OFF)

The data range of this particular parameter differs, depending on if you are running the machine in Metric or Inch Mode.

 

For Metric, the valid range is 30-240000, and for Inch, the range is 30-96000.

 

The "units" for the Inch Mode are in ".1 Inch/Min", which means a value of "30" would be "3.0 IPM". So if you used "96000", that would equate to "9600.0 IPM", which is most likely greater than your actual "max rapid rate". Make sure you know the original value before you begin. In the above example, "R6000" equates to "600.0 IPM", for the Z axis.

 

So technically, you can turn down the rapid traverse rate from inside the NC Program, cut the hole using the slow retracts, then set the rapid traverse rate right back to the default. No operator intervention required...

[Newbeeee™]

Colin - I didn't realise you could do this mid prog.

Every day's a school day!

[Machineguy]

Rqpid override on the machine. I use it on the lathe, a lot. Gives a chance for the tool to cool off and flush the chips off the drill. Mainly for deep drilling of 35% glass filled nylon.

[AMCNitro]

If you still want to use a Canned Cycle to drill your holes, instead of having to resort to "long-hand" output, you could also just slow down the Rapid Rate of your machine.

 

This can be done easily by Programmable Data Entry. First, make sure you write down the "default" value of the parameter before you change it!

 

The Rapid Traverse Rate on most Fanuc controls is parameter #1420. This value is a two-word axis parameter (also known as a long integer). That means that the individual address (XYZABC) is set using a "P" number, and the "R" value that follows is an integer (some are signed, these are not!). Depending on the "increment" of the input, the "range" will differ.

 

You can use a Manual Entry toolpath to insert this code as G-Code, directly into your program:

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P1 R500
N1420 P2 R500
N1420 P3 R500
G11
(PARAMETER ENTRY MODE OFF)

In the above example, I'm setting X, Y, and Z rapid traverse rate to 50.0 Inches per minute.

 

We can do the same thing, and only set the Z axis instead, like so:

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P3 R500
G11
(PARAMETER ENTRY MODE OFF)

Then, after the drilling operation is complete, we can set it back to whatever the "default" value is, but remember that we first have to know what the original value was before starting!

G90
(PARAMETER ENTRY MODE ON)
G10 L50
N1420 P3 R6000
G11
(PARAMETER ENTRY MODE OFF)

The data range of this particular parameter differs, depending on if you are running the machine in Metric or Inch Mode.

 

For Metric, the valid range is 30-240000, and for Inch, the range is 30-96000.

 

The "units" for the Inch Mode are in ".1 Inch/Min", which means a value of "30" would be "3.0 IPM". So if you used "96000", that would equate to "9600.0 IPM", which is most likely greater than your actual "max rapid rate". Make sure you know the original value before you begin. In the above example, "R6000" equates to "600.0 IPM", for the Z axis.

 

So technically, you can turn down the rapid traverse rate from inside the NC Program, cut the hole using the slow retracts, then set the rapid traverse rate right back to the default. No operator intervention required...

I've always wondered if there was a way to override the rapid IN the program separate from the machine overrides(5%, 25%, 50% and 100%), I even spoke to a Haas applications engineer.  Thank you Sir!! Ill look at these when I have a bit more time.

 

Rqpid override on the machine. I use it on the lathe, a lot. Gives a chance for the tool to cool off and flush the chips off the drill. Mainly for deep drilling of 35% glass filled nylon.

Yes, but then you have to leave at the override and the machine will run slower, or worse, you need to have a guy set overrides on each operation.

[Machineguy]

Yea, I know. but this is a 2 man shop.

[Colin Gilchrist]

Yea, I know. but this is a 2 man shop.

Even in a 1 man shop, the solution I posted means you don't have to babysit the machine. You program the override reduction right into the NC code. That way you also don't have to "remember" any special process instructions when the job repeats in 6 months.

[AMCNitro]

Yea, I know. but this is a 2 man shop.

Its just me here 

[mkd]

Its just me here 

^^me too^^

 

not to rain on the above awesome fanuc solution, but Haas won't take a G11. I'm totally clueless if there is a parameter to control rapid speed or if it can be set through a program. interested to see what Haas AE says about this cool possibility.

 

X0 Y0

M97 P100

X10.Y5.

M97P100

..

..

M30

N100

G91Z-.5F10.

Z.5F50.

G90

M99

 

ONE CLUNKY WAY^^^..

 

better to setup a custum G code in the haas control to call my subprogram as a '9000' program (like JParis said)

[Colin Gilchrist]

It would have to be a one-line G10 entry. I don't know if it will work, but you could try something like:

 

G10 L50 G90 Nxxxx Px Rxxxxxxxx

 

I just don't know if Haas built this capability into their controls. It would sure be a shame if it wasn't possible, since they do support so much of the "standard Macro B" functionality OOTB. They have enough capability to integrate probing into their controls, so I would assume this is somehow possible, if we can get the correct info from Haas...

[A.MAHLER]

You can use the G85 canned cycle, It does a feed retract.

[MIL-TFP-41]

One thing to note using Colin's method, which is a great idea BTW, on the newer 30i controllers to do parameter entry in a program you have to use "G10 L52"

You can do tons of things with this...

[Colin Gilchrist]

There are all kinds of cautions and differences in how the Parameters are formatted for a particular control model. Like most complex systems, a Fanuc controller can be ordered with different options.

 

There are different "Memory Types". A/B being the most common, but some machines have Memory Type C. Depending on the A, B, or C type, the range of the variable can be different. Also, the input increment (Base Unit) can vary. (some values might be specified in .0001 inch units for memory type A/B, but for memory type C, the base unit might be .00001.)

 

In addition to Memory Type, the "Units" setting of the control (Inch vs. Metric) comes into play, because the Unit Type Setting changes the range of the allowed input values.

 

Finally, the Data Type itself has to be known. There are four discrete data types:

 

Bit

Byte

Word

Two-word

 

Bit types have a Range of 0 or 1

Byte types have a Range of 0 to +-127 or 0-255 (byte axis)

Word types have a Range of 0 to +-32767

Two-word types have a Range of 0 to +-99999999

 

So you must know not only what parameter number you want to manipulate, but the data type, and data range of the variable in question.

 

For the basic "Two-word" type, the allowable Range is + or -, eight-nines. (+-99999999), however, for each parameter in use by the machine builder, that basic "range" can be restricted.

 

For the "Max Rapid" parameter #1420, on a Fanuc 18, the range is as follows:

 

On a machine with "A/B" Memory type: for Metric, the valid range is 30-240000, and for Inch, the range is 30-96000

 

So as you can see, the "data range" of eight-nines, has been limited to 240,000 for Metric, and 96,000 for Inch mode. (These range limits change for a machine that has Memory Type C.)

 

So there are quite a lot of considerations to keep in mind when learning about Programmable Data Entry, but the results are very much worth the effort to learn.

 

I highly recommend picking up a copy of Peter Smid's book: FANUC - CNC Custom Macros; Programming resources for Fanuc Custom Macro B users.

 

http://www.amazon.com/Fanuc-Custom-Macros-Peter-Smid/dp/0831131578/ref=sr_1_3?ie=UTF8&qid=1453908195&sr=8-3&keywords=peter+smid

 

There are other books on the market with similar content, I also have the one by S.K. Sinha: CNC Programming using Fanuc Custom Macro B.

 

http://www.amazon.com/Programming-using-Fanuc-Custom-Macro/dp/0071713328/ref=sr_1_1?ie=UTF8&qid=1453908252&sr=8-1&keywords=macro+b

 

Both are excellent resources...

[Machineguy]

^{I don't see a macro override for the rapid in the Haas. Looks like a custom macro is needed.}

[Newbeeee™]

One thing to note using Colin's method, which is a great idea BTW, on the newer 30i controllers to do parameter entry in a program you have to use "G10 L52"

You can do tons of things with this...

Not just the 30i controls.

Also the 0iD and latest 0iF (which is a cut-down 30 series).

 

Edit: 0iC (B and A) is 16/18/21 series so works with L50

[Colin Gilchrist]

Yes, I'm not sure what the cutoff date was. The Fanuc 15, 16, and 18 series, and my Oi-TC controls use L50. Many newer versions use L52.

 

The syntax of the operation will almost always be flavored by your particular control model. The key is to get a hold of the parameter manual, and programming manual, to see what the format is for your specific configuration.