The Collected Wisdom
of the Haas Answer Man

Programming

(early 2005
vol 9 # 32)

Dear Applications:

I’m a machining technology student at a community college. My latest assignment for the Haas CNC class involves pocket milling with G150. I put in G and M codes like the program in the workbook, and it worked fine on the simulator. Then my instructor and I tried another program, which is very simple but won’t work. Maybe you could look at this and tell us what’s wrong? Thank you.

Dave Martin
 

Dear Dave:

Your program is fine until the next-to-last line.

(early 2005
vol 9 # 32)

Dear Applications:

How do I program helical milling in the Z axis? Do I have to loop circular interpolation with a Z value added for each revolution (G02 X__, Y__, I__, J__, Z__)? Or is there a G code for helical milling or interpolation in the Haas control?

Chuck Wong

Dear Chuck:

The simplest way to achieve helical motion is by X and Y circular interpolation (G02 or G03) with a Z value added per revolution. Use an I command to specify the distance in X from the starting point to the center of the arc. To cut a complete circle of 360 degrees, do not specify an ending point for X or Y. If you use incremental positioning (G91), you can loop the cycle to achieve your depth using an L command. Here’s a sample program:

%
O1234;
(Helical Milling Example);
T1 M06;
G00 G90 G54 X0. Y0. S3000 M3;
G43 H01 Z0.1;
G00 X0.5;
G91;                                          (incremental positioning)
G02 I-0.5 Z-0.25 F20. L4;       (helical motion, 1 in. dia. x 1 in. deep)
G00 G90 X0;
G0 Z0.1 M09;
G53 Z0.;
G53 Y0.;
M30;
%

Sincerely,
Haas Applications

(early 2005
vol 9 # 32)

Dear Applications:

I’m using G47 to engrave serial numbers, but I’m getting error message number 529: “Illegal G65 parameter. The addresses G, L, N, O, and P cannot be used to pass parameters.” What can I do to fix this? Here’s my program.

G47 P1.0 (5001) X0.5 Y0.75 J0.125 R0.05 Z-0.005 F25.0 E10.0

Thanks for your help.

Vijay Bakshi
 

Dear Vijay:

You need to take the decimal point out of the P command – in this case, P is an instruction (Engrave Sequential Numbers) rather than a value, so “P1” is the correct form of the command.

Sincerely,
Haas Applications

(Fall ’04
vol 8 # 31)

Dear Applications:

I need to do circular milling on my VF-3. I would like to know about I and J moves – how are they calculated? Are I and J arc segments of the circle?

Rod Lewis

Dear Rod:

The optional I, J and K commands represent the distance from the starting point to the center of the circle: I is the distance along the X axis; J is the distance in Y; K the distance in Z. (Typically, I and J are used in mill programming, while I and K are used with lathes.) Depending on your application, the R command may be used instead.

If you’re cutting an arc of less than 360 degrees, you should use X, Y, Z and R commands. The X, Y and Z values define the endpoint – which is different from the starting point – and the R value is the distance from the starting point to the center of the arc. Note that if R has a positive value, the control will generate a path of 180 degrees or less; to generate an arc of greater than 180 degrees, you must specify a negative R.

To cut a complete circle – a 360-degree arc – you must use I, J, K commands (if only one of these values is specified, the others are assumed to be zero). In this case, the starting point and ending point are the same, so you don’t need to specify X, Y or Z values.

Sincerely,
Haas Applications

(Summer ’04
vol 8 # 30)

Dear Applications:

I have a question about one of the programming examples in your operator’s manual. Here’s the example in question:
  T200 B-2.0 
  G50 S2500 
  G97 S1042 M03
  G00 G99 X2.0 Z0.01
  T232 M08 
  G96 S600 
  G01 Z0 F.01

     What is the purpose of the program line that has G97 S1042 M03 in it? I ask because of the G96 S600 code that follows two lines down in the program. This just doesn’t make sense to me. Thanks.

     Joe Killeen
 

Dear Joe:

When you invoke G96, Constant Surface Speed (CSS), the machine will automatically increase or decrease spindle speed according to the radius being cut (distance from tool tip to spindle centerline). This is an excellent way to ensure the proper cutting speed for the material being used. The common practice is to program with G97 (turn off CSS) when rpm adjustment is not necessary, such as during any rapid moves to approach the part or during drilling. A G96, with its increasing or decreasing speed, can sometimes be inconvenient during non-cutting moves. For example, if your programmed feed is in inches per rev and the tool tip moves outward, everything will slow down – and your cycle time will increase.
    In conclusion: Use G96 only during cutting, and cancel it as soon as possible with a G97 command.

     Please feel free to contact us for further assistance.

     Sincerely,
     Haas Applications

(Spring ’04
vol 8 # 29)

Dear Applications:

I have a question about subroutines on my VF-6. I want to mill the same contour in several places – a 10 x 10 mm rectangle, repeated 100 times. What’s the best way to do this?

     Gunnar Gustavson

Dear Gunnar:

     It’s pretty easy. Here is an example, in inches, of calling an incremental (G91) pocket subroutine from within a main program.

     TIP: Your machine [given serial number] has a powerful Haas option that allows you to manipulate subroutines using rotation and/or scaling. You will still have to program the subroutine in incremental mode. With this option enabled, G68 commands rotation at any angle from the designated center of the part or from the subroutine zero point, and G51 controls scaling. Your operator’s manual has details on the correct use of these G codes, or you can contact us for further assistance.

     Sincerely,
     Haas Applications

(Fall ’03
vol 7 # 27)

Dear Applications:

I am trying to run a 3D program on my VF-3. It’s too big to fit on a floppy, and we cannot send files from PC to Haas yet. Is there a way that I can take the three programs that actually make up one part and combine them on the Haas? I am looking for a way I can run this part overnight, without having to come in and call up another program.

     Dave Bartlett
 

Dear Dave:

Yes, you can combine your three programs easily. Make a cover program like this:

  O0001;
  M98P101;       (first sub-program number is O101)
  M98P102;       (second sub-program)
  M98P103;       (third sub-program)
  M30;

     Be sure to put an M99 instead of an M30 at the end of each sub-program, so that it will return to the cover program.

     Sincerely,
     Haas Applications