[Hobgoblin]

For the purpose of this question I will use this example.

I have a infinate steel slab, which i want to drill a circle patter on holes.

36 holes, 20mm hole diameter (irelevant i suppose but for completeness...), 1000mm Pitch Core Diameter. 100mm deep.

using this machine, in which X axis is 12,000mm long, the Y axis is 3000mm up and down (vertical), and the Z axis 1500mm is the movement of the ram in and out.



Now, using G16, with G18 i have made a program like this,
O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
Z500 X10
Z500 X20
Z500 X30
Z500 X40
... Etc untill ...
Z500 X350
G15

BUT, AND THIS IS THE REASON I AM HERE,

how about
O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
G15
G65 P2 L35

where O0002 is:

O0002
G91
G16
Z500 X10
G15
G90
M99


The first program i did similar today at work on such machine, and tried the second but was unsucessful, but rather than mess i got on, did the job, and am here now for advice for the future.

wondering if it will work without the Z500?
O0002
G91
G16
Z500 X10
G15
G90
M99

My aim is just to reduce lead times by not having to work out or enter the Z & X positions for each hole (the old fashioned way). But even tho i think polar is faster, it still takes time writing 35 lines of increasing 10degrees each time, which is why i was wanting to combine the polar program, with a program to further reduce times.

Any suggestions?

[txcncman]

I think you could accomplish this best by using incremental moves and coordinate rotation both inside your sub-program. Then change back to normal coordinates with absolute after return from your sub-program.

[Hobgoblin]

I think you could accomplish this best by using incremental moves and coordinate rotation both inside your sub-program. Then change back to normal coordinates with absolute after return from your sub-program.

Could you show me an example of what you mean with code?

thanks for your help

[angelw]

For the purpose of this question I will use this example.

I have a infinate steel slab, which i want to drill a circle patter on holes.

36 holes, 20mm hole diameter (irelevant i suppose but for completeness...), 1000mm Pitch Core Diameter. 100mm deep.

using this machine, in which X axis is 12,000mm long, the Y axis is 3000mm up and down (vertical), and the Z axis 1500mm is the movement of the ram in and out.



Now, using G16, with G18 i have made a program like this,
O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
Z500 X10
Z500 X20
Z500 X30
Z500 X40
... Etc untill ...
Z500 X350
G15

BUT, AND THIS IS THE REASON I AM HERE,

how about
O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
G15
G65 P2 L35

where O0002 is:

O0002
G91
G16
Z500 X10
G15
G90
M99


The first program i did similar today at work on such machine, and tried the second but was unsucessful, but rather than mess i got on, did the job, and am here now for advice for the future.

wondering if it will work without the Z500?
O0002
G91
G16
Z500 X10
G15
G90
M99

My aim is just to reduce lead times by not having to work out or enter the Z & X positions for each hole (the old fashioned way). But even tho i think polar is faster, it still takes time writing 35 lines of increasing 10degrees each time, which is why i was wanting to combine the polar program, with a program to further reduce times.

Any suggestions?

The radius value set in the G81 cycle (Z500.0) is modal and therefore does not have to be specified continually in the Sub Program. In the Sub Program you can specify an incrementally applied angle and have the Sub repeat as many times as required. I note that you're calling O0002 with the Macro Program call G65, any reason for that?

Is your program example as its registered in the control? Unless the control is set up in Pocket Calculator mode, coordinates specified without periods will be treated as the number of least programmable increments. For example, in Metric mode Z500 will be interpreted as Z0.500.

Also, I wouldn't continually start and cancel Polar Coordinate Command in the Sub. You could try something like the following:

Regards,

Bill

O0001
G90
S716 M3
M7
G00 X0.0 Z0.0
G43 H1 Y100.0
G16
G98 G81 Z500.0 X0.0 Y-100.0 R5.0 F143
M98 P2 L35
G15 G80
.........
.........
.........
M30
%

%
O0002
G91 X10.0
M99
%

[lshingleton]

If you have Macro B on the machine try this one



O0001
G00G90X-10.0Z500.0G43H1Y25.0M3S716
M7
()
G00Y5.0
()
#500=37.0 (NUMBER OF HOLES PLUS ONE FOR FIRST LOCATION)
#501=10.0 (X-AXIS MOVEMENT OR SPACING BETWEEN HOLES)
()
WHILE[#500GT0]DO1
()
G01G91X10.0F#530
G90
()
G98 G81 Y-100 R5 F#531
()
#500=[#500-#501]
END1
()

MOVE HOME

[txcncman]

You state "circle pattern of holes". I assume you mean like represented in the attached screen shot. Your sample program X, Y, and Z moves do not match with the description of your machine axis movement.

[angelw]

You sample program X, Y, and Z moves do not match with the description of your machine axis movement.

I believe it does, as the OP states that he's specifying the drilling plane with G18 (drilling using the Y axis). Therefore Z and X are the respective
addresses for the radius and angles used in polar coordinates.

Regards,

Bill

[lshingleton]

O0001(BOLT CIRCLE)
()
G00G90G54P1X0.0Z0.0G43H1Y25.0M3S716
M7
()
G00Y5.0
()
(CIRCLE REQUIREMENTS)
#20=100.00 (PCD)
#11=36 (# OF HOLES)
#15=0 (START ANGLE)
()
(CIRCLE CALCULATIONS)
#16=[360/#11](ANGLE BETWEEN HOLES)
#14=[#20/2] (RADIUS)
()
WHILE[#11GT0]DO1
#5=#14*SIN[#15]
#6=#14*COS[#15]
()
G00X#5Z#6Y5.0
()
G98 G81 Y-100 R5 F#531
()
#15=[#15+#16]
#11=#11-1
END1
()

MOVE HOME

If your running a true bolt circle and not straight line this one will work for any fanuc control and any number of holes----

[txcncman]

I believe it does, as the OP states that he's specifying the drilling plane with G18 (drilling using the Y axis). Therefore Z and X are the respective
addresses for the radius and angles used in polar coordinates.

Regards,

Bill

Was just trying to clarify. I did not see that he is using an angle attachment on the spindle for drilling. Once the basic cycle is established, it can easily be translated to any plane.

[Hobgoblin]

I note that you're calling O0002 with the Macro Program call G65, any reason for that?

My mate who works the nightshift on the same machine uses m98, i was just learned g65 first and have stuck with it. I dont really know any other way, im pretty new to fanuc (3 months self taught expirience) but i have a good knowlege of heidenhain and machining in general.

Is your program example as its registered in the control? Unless the control is set up in Pocket Calculator mode, coordinates specified without periods will be treated as the number of least programmable increments. For example, in Metric mode Z500 will be interpreted as Z0.500.

i dont understand your first sentence here, but we only use metric (rarely use english and even then we convert to metric). When I write Z500, Z Would move 500mm, if it were g91 ofcourse.

Also, I wouldn't continually start and cancel Polar Coordinate Command in the Sub. You could try something like the following:

That makes so much sense, i havent tested it but it looks like it should work. next time im doing a PCD of holes i will test this method out.

You state "circle pattern of holes". I assume you mean like represented in the attached screen shot. Your sample program X, Y, and Z moves do not match with the description of your machine axis movement.

I mean that I am drilling in the y Axis, and there is a circular pattern of holes in the Z X planes, which the circle centre is z0 x0.

O0001(BOLT CIRCLE)
()
G00G90G54P1X0.0Z0.0G43H1Y25.0M3S716
M7
()
G00Y5.0
()
(CIRCLE REQUIREMENTS)
#20=100.00 (PCD)
#11=36 (# OF HOLES)
#15=0 (START ANGLE)
()
(CIRCLE CALCULATIONS)
#16=[360/#11](ANGLE BETWEEN HOLES)
#14=[#20/2] (RADIUS)
()
WHILE[#11GT0]DO1
#5=#14*SIN[#15]
#6=#14*COS[#15]
()
G00X#5Z#6Y5.0
()
G98 G81 Y-100 R5 F#531
()
#15=[#15+#16]
#11=#11-1
END1
()

MOVE HOME

If your running a true bolt circle and not straight line this one will work for any fanuc control and any number of holes----

Hi thanks for a different perspective here, Ive not done parameter programing before for a fanuc, I have done some for a heidenhain. I can make sense of what your aim with the code is here, but am struggling to understand confidently the science/method of how its working. (baby talk welcome, if your willing to help it sink in to my head a bit easier)

Was just trying to clarify. I did not see that he is using an angle attachment on the spindle for drilling. Once the basic cycle is established, it can easily be translated to any plane.

Hi the machine is fitted with a 2axsis head, the rear rotates 360degress and the front head rotates 180 degrees, im not sure if thats relevent for the example though, if we just assume im using g18.


thanks for all help so far

//EDIT//
Just realising there might be a language barrier accross the pond. When i say PCD of holes, or circular hole pattern im meaning what you may know as a bolt circle, or bolt hole pattern.

[txcncman]

The technique I was suggesting would be use absolute mode to move to the center of the bolt hole circle pattern. Then call a sub-program. The sub-program would be incremental to rotate the work coordinate system, move to the location of a hole, drill the hole, then move back to the center of the bolt circle pattern. Should look something like this:

O0001
G90
S716 M3
M7
G00 X0.0 Z0.0
G43 H1 Y100.0
G18
M98 P2 L36
G69
G90
G17
...
...
...
M30
%

%
O0002
G91 G68 X0. Z0. R10.
G91 X500.
G90 G98 G81 Y-100.0 R5.0 F143
G80
G91 X-500.
M99
%

[ChattaMan]

Why bother with a sub. To use the least amount of code repeat with K

O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
G91 X10 K35
G80 G90 G15

This will increment by 10 degrees 35 times.

:banana:

[lshingleton]

I have programmed for awhile and dont recommend some of these
The G65 code is an easy one but has issues in that it changes specfic codes in fanuc to mean othere things thus the danger
M98P2000------best way to call a sub for anything
macro programing the easiest but sometimes not available on older machines
()
This machine seems to have a problem in that the spindle vertical axis moving to part is Y axis not Z---------someone has done something along the way or machine builder not following any standard
In the program i showed you it uses G54 p1 xo yo ----this is picking up the center of the bolt circle and is common practise -------some older machines only have G54/55/56/57/58/59 but newer one go up to G54 P48 giving over 50 work offsets for one part
The G68 and G69 we only use to rotate a center to casting or loaction point on a mill-----must be used with caution becasue sometimes fails to cancel---or must be set in the parameters to cancel at reset or power on and i mean sometimes 1--in 10000 but the once can be enough

[txcncman]

Why bother with a sub. To use the least amount of code repeat with K

O0001
G90
S716 M3
M7
G00 X0 Z0
G43 H1 Y100
G16
G98 G81 Z500 X0 Y-100 R5 F143
G91 X10 K35
G80 G90 G15

This will increment by 10 degrees 35 times.

:banana:

I missed the G16. I stand corrected.

[angelw]

My mate who works the nightshift on the same machine uses m98, i was just learned g65 first and have stuck with it. I dont really know any other way, im pretty new to fanuc (3 months self taught expirience) but i have a good knowlege of heidenhain and machining in general.

The major difference between using G65 and M98 is that arguments are able to be passed to the program being called when G65 is used, whereas this is not possible when using M98. In your example, you're not passing any arguments, only calling the program and having it repeat a number of times

Following is an example of a Bolt Hole Macro, where arguments are being passed to it when called by either G65 or an example Custom G code (G100).

From the main program, the following block will call Macro program O9010 and pass the values to Local Variables that correspond to the addresses X, Y, R, Z, F, I, A, B, and H

Call block using G65
G65 P9010 X100.0 Y50.0 R30.0 Z–50.0 F500 I100.0 A0 B45.0 H5

The G65 can also be replaced with a Custom G code. For example, if the number 100 is registered in parameter 6050 (late series Fanuc control), program number O9010 will be called when G100 is specified in your program.

The call block would then be:

Call block using Custom G code (G100)
G100 X100.0 Y50.0 R30.0 Z–50.0 F500 I100.0 A0 B45.0 H5

Where:
X: X coordinate of the centre of the circle
(absolute or incremental specification – local variable #24)
Y: Y coordinate of the centre of the circle
(absolute or incremental specification – local variable #25)
Z: Hole depth (local variable #26)
R: Coordinates of an approach point (local variable #18)
F : Cutting feedrate (local variable #9)
I : Radius of the circle (local variable #4)
A: Drilling start angle (local variable #1)
B: Incremental angle (clockwise when a negative value is specified local variable #2)
H: Number of holes (local variable #11)


O9010;
#3=#4003 Stores G code of group 3.
G81 Z#26 R#18 F#9 K0
Note 1: Drilling cycle - no execution happens at the initial point due to the K0.
Note 2: L0 can also be used.
IF[#3 EQ 90]GOTO 1 - Branches to N1 in the G90 mode.
#24=#5001+#24 - Calculates the X coordinate of the centre.
#25=#5002+#25 - Calculates the Y coordinate of the centre.
N1 WHILE[#11 GT 0]DO 1 - Loop until the number of remaining holes reaches 0
#5=#24+#4*COS[#1] - Calculates a drilling position on the X–axis.
#6=#25+#4*SIN[#1] - Calculates a drilling position on the Y–axis.
G90 X#5 Y#6 - Performs drilling after moving to the target position.
#1=#1+#2 - Updates the angle.
#11=#11–1 - Decrements the number of holes.
END 1
G#3 G80 - Returns the G code to the original state.
M99

The above Macro is not limited to having the centre of the PCD at X0 Y0. The coordinates for the centre are passed as either Absolute or Incremental values via arguments X and Y in the Macro Call block.

Once the PCD Macro program has been registered in the control, any PCD configuration can be conveniently programmed by including the required PCD data in the Macro call block.

i dont understand your first sentence here, but we only use metric (rarely use english and even then we convert to metric). When I write Z500, Z Would move 500mm, if it were g91 ofcourse.

Generally, the default parameter settings of a Fanuc control requires a period (decimal point) to be included in the various addresses, such as X, Y and Z for the value to be interpreted correctly. The parameter and bit for Fanuc controls such as Series 16i, 18i, 21i, Oi etc, to determine this is #3401.0

1. If this bit is set to Zero (default), then the least input increment is assumed and a decimal point is required for addresses such as X, Y and Z, to be determined correctly. In this case, X500 would be interpreted as X0.500 (metric system)
2. If this bit is set to 1, then the unit of mm, inches, or second is assumed. Fanuc refer to this as Pocket calculator type decimal point input. In this case X500 will be interpreted as X500.0

If G91 X500 moves your machine's X slide 500mm, then clearly your control has been set in Pocket Calculator format.

Regards,


Bill

[angelw]

This machine seems to have a problem in that the spindle vertical axis moving to part is Y axis not Z---------someone has done something along the way or machine builder not following any standard

This is not unusual with this style of machine, where it can be configured as a Vertical or Horizontal machine. The OP has pointed out that the machine has a two axis head.

Correct. This code will repeat the X10. move 35 times and make a straight line of holes.

In ChattaMan's example, where Polar Coordinates has been made active with G16, the repeat of the drilling operation will be in 10degree increments at a radius of 500mm, not in a straight line

Regards,

Bill

[lshingleton]

Bill
We have 7000 CNC machines and thats a small estimate and never moved a vertical spindle to a part on a Y axis---------some really smart maintenace and machine builder applications guys have been known to play with drive conections/parameter config and what ever to make stuff run so rare i will stick with
The rest of the stuff is spot on but i would have to say way over the head of most laymen cnc machinist in our shop today ----remember the KISS rule---KEEP IT SIMPLE STUPID our you will be going back often to fix it yourself and when Murfey is around it would most likely be at 4 am on a sat
()
best of luck guys with the programming

[angelw]

Bill
We have 7000 CNC machines and thats a small estimate and never moved a vertical spindle to a part on a Y axis---------some really smart maintenace and machine builder applications guys have been known to play with drive conections/parameter config and what ever to make stuff run so rare i will stick with
The rest of the stuff is spot on but i would have to say way over the head of most laymen cnc machinist in our shop today ----remember the KISS rule---KEEP IT SIMPLE STUPID our you will be going back often to fix it yourself and when Murfey is around it would most likely be at 4 am on a sat
()
best of luck guys with the programming

The number of machines you have is irrelevant. Machines where drilling operation can occur in various axes abound. Many 5 axis machines are so constructed to be able to do this via program command to move the spindle head to a new orientation, and any 3 axis Machining Centre, vertical or horizontal, can do this by merely using a 90deg angle tool holder, of which there are many.

What part of my PCD Macro is more hard to understand that your example?

The only additional explanation I've made is regarding the use of G65, and if you're going to learn Macro Programming techniques, the way in which Macro Programs are called is one of the first things to learn. The fact is, by using a G65 or a Custom G code command line to call the Macro makes for a much more user friendly program. All of the edits required to reconfigure the PCD machining code are contained in one block, whereas in your example the editing is spread over a number of blocks, including the edit required in the G81 cycle.

But getting back to the OP's original question, using G16 to activate Polar Coordinates is probably the cleanest way, whether used in a Sub Program, or with a repeat argument in the drill cycle command, as suggested by ChattaMan, for him to proceed. The next best would be a Macro Program, similar to my example, registered in memory and called when required, passing the required arguments to the Macro so as to obtain the desired PCD and drilling configurations.

Regards,

Bill

[lshingleton]

Number of machines is very realevant in making a statement of common/uncommon
The Program i used has no G65 thus no changing of Letter values---No special G100-to whatever codes forund from 6050 to 6081 parameter numbers
()
If you read his program there is no work offset so that would be a start for learning these guys
()
But you must be an aplications guy becasue you dont see how advanced it is or how much people dont know because of training
i could program in Qbaisc -onvert all the letters-----call every parameter in the machine and mutiply them by macros no one sees but why would i

Remeber guys to Start with the basics and pay more attenshion to program structure than fancy stuff
Stick to the M98/M99s and stuff like that till your sure of what your doing
CNC machines are not like computers-when they crash it is very dangerous for the operator and can cost millions to fix

[angelw]

Number of machines is very realevant in making a statement of common/uncommon

Of course its irrelevant. A shop could be a total turning shop having a vast number of turning centres. On your criteria, that shop would consider machining centres rare. Just because you don't have the type of machine described by the OP doesn't mean they don't exist, or that they're rare. I reiterate, machines that are able to drill using the Y axis abound, it just seem you're not yet aware of them.

The Program i used has no G65 thus no changing of Letter values---No special G100-to whatever codes forund from 6050 to 6081 parameter numbers

So are you calling your program as a Sub Program, or is it in the Main Program?

If a Sub Program, every time a change to the PCD, or drilling cycle configuration needs to be made, you have to seek out that program, make the changes in more than one block and return to the Main Program.

If in the Main Program, and if the pattern is to be repeated elsewhere, you have to copy all of your program, or provide GOTO and Conditional statements to jump from place to place. That clearly is more difficult for a newbie to understand than a single block G65 call statement.

In the example I gave, you simply have to edit the numerals associated with the component of the Macro Program you need to alter, and its all in one block.

If the PCD function needs to be repeated in anther place, you have one block only to copy elsewhere in the program.

The OP's criteria that I comprehended, was that he wanted to save time in the process of creating the program. I think editing one G65 block at a time achieves that, should he go the Macro way.

If you read his program there is no work offset so that would be a start for learning these guys

The topic of this thread related to the Polar Coordinate function G16. Many who list programs on this and many other forums frequently don't Copy and Paste their code and leave out much. The OP stated he was able to achieve a result with what he had and was asking for suggestions regarding the code he had in regards to Polar Coordinate programming. Work Shift programming is for another day.

But you must be an aplications guy becasue you dont see how advanced it is or how much people dont know because of training

If you consider that the one G65 block in my example is advanced, or difficult to understand, particularly given the legend for the addresses used, then you have much to learn. Apart from the example PCD Macro I listed being far more flexible than the one in your example, the complexity (simple) of the two are similar. As far as the use of G65 to call and pass arguments to be used by the Macro Program is concerned, that is Greasy Kid Stuff. I see first year apprentices in the many shops I'm associated with, using that structure as simply as if writing a canned cycle block.

Remeber guys to Start with the basics and pay more attenshion to program structure than fancy stuff
Stick to the M98/M99s and stuff like that till your sure of what your doing
CNC machines are not like computers-when they crash it is very dangerous for the operator and can cost millions to fix

Yes, I agree that one shouldn't get out of one's depth. However, there is nothing fancy about calling a Macro Program with G65. I tend to give people credit for intelligence.

Regards,

Bill