Answers to Your Questions

 

 

 

 

 

 

 

 

 

 

 

 

   

The Collected Wisdom
of the Haas Answer Man
   

Higher Productivity Made Easy
 

 

Counting Parts per Bar

(early 2005
vol 9 # 32)

Dear Applications:

I’m using a bar puller with my SL-20, and each bar gives me 32 parts. I have a main program and a sub-program, and the sub-program ends with M99. Is there a page or screen on the control that shows what the part count is at any point in the M98 L32 loop? I found the M30 count in Current Commands, but that doesn’t tell me where I’m at in my 32-piece bar. Setting 118, M99 Bumps M30 Counters, doesn’t work when the M99 is in a sub-program. Can you help me? Thanks.

Mike Hernandez

Dear Mike:

Page up to the Tool Life screen in Current Commands, and monitor the USAGE count for the bar puller tool number. If you don’t have the Macro option on your SL-20, you’ll need to manually zero out the Usage column for this tool number at the beginning of each bar (cursor onto it and press the ORIGIN key). With macro variables, you could do that via the part program – or you could program an instruction that will bump the M30 counter at a sub-program M99.

Here’s a sample program, using macros, that we have used to count parts on M30 counter #1 and count bars on M30 counter #2. Setting 118 may be either on or off.

%

 

O00001

(Main program)

#1=0

 

N1

 

M98 P100

(sub-program call)

#3901=#1

(tells machine to count M99s on counter #1)

#1=#1+1

(add 1 to the counter every time program is run)

IF [ #1 EQ 32 ] GOTO2

(repeat program 32 times)

GOTO1

(go to N1 until #1 = 32)

N2

 

M30

(these will be counted on counter #2)

%

 

 

%

 

O00100

(Sub-program)

N10
G28
T101
G97 S500 M03
G00 X2.0 Z.1
Z0
G01 X1.9 F.010
G00 Z1.0 M05
G28
M99
%

Sincerely,
Haas Applications

• • •

Haas Servo Bar 300 –
Programming

(Fall ’04
vol 8 # 31)

Dear Applications:

We just got an SL-20 lathe with a Servo Bar 300. I set macro variables 3100, 3101 and 3102 to zero, because a coworker told me I should remove the bar feeder settings so that we won’t have any problems with our existing programs. Are these the only variables I need to worry about? Enclosed is the first program I want to run. What else do I need to check or verify before I run it?

Rick Schumacher

Dear Rick:

You’re using I, J and K commands on the G105 (Servo Bar Command) line in your program. These IJK codes will override the macro variables, so – although it certainly doesn’t hurt – it is not necessary to set the variables to zero.

Please check the numbers in your program, however. Macro variable 3100 corresponds to the letter J, variable 3101 corresponds to the I value, and 3102 is the letter K. Make sure that these values are in the right order.

Regardless of whether you use macro variables or IJK values, you still need to use G105 Q4 and G105 Q2 commands to set a reference position. The best method for setting a reference position uses a known location such as the chuck or collet face. Before you begin, check for proper spindle liner size, bar clamp adjustments and transfer tray alignment.

Macro variable #3112, Reference Position, is established during setup but is not entered by the operator. Once the reference position is set, it remains the same for any other bar diameter or part length. It only needs to be reset if the bar feeder is moved or if it must be changed to fit a new collet or chuck setup.

You must enter values for the three bar feeder macro variables described below. (You can zero them later if you want to.) You’ll find them in the Current Commands display; PAGE DOWN to the “Haas Servo Bar” screen, then use the up or down arrow keys to highlight the variable. Type in the value and press WRITE/ENTER.

#3100, Part Length + Cutoff, is the bar length pushed out at each G105 command after the bar is loaded. It’s equal to finished part length plus cut-off and face clean-up allowance.

#3101, Initial Push Length, is the distance past the reference position to which each new bar will be pushed when it is loaded.

#3102, Min Clamping Length, is the bar length required to support the

length that will be pushed out past the
chuck or collet face. This depends on bar diameter, part length and initial push length.

Here are the steps for setting reference position.

1.

Enter a value for macro variable #3101.
2.

Enter a value for macro variable #3102.
3.

Place a bar on the charging tray.
4.

In MDI mode, enter G105 Q4 and then press CYCLE START. The machine will load the bar, pushing it into the lathe so the lead end is about 4 inches away from the cutting area.
5.

Press RESET, to enable bar feed using the jog handle.
6.

Select the V axis by pressing the V key; then press HAND JOG. Using the jog handle, push the bar up to the chuck face or collet face to be used as the reference point.
7.

Clamp the bar.
8.

In MDI mode, enter G105 Q2 and then press CYCLE START. The machine will use the bar position to enter a value in macro variable #3112, unclamp the bar, push it out by the amount set in variable #3101, and reclamp.

Please read your Servo Bar  Operator’s Manual for more detailed instructions.

Sincerely,

Haas Applications

• • •

Haas Servo Bar 300 –
Alternating Pushes

(Summer ’04
vol 8 # 30)

  

Dear Applications:
      We need to know about your bar feeder. Can it make two different, alternating pushes? I need to turn 2-inch–long and 3-inch–long pieces from the same bar stock. Can I alternate them?
     Clark Crenshaw

 
Dear Clark:
      Yes, you can do multiple bar pushes with the Haas Servo Bar 300. The I, J, and K commands will override the macro variables for the program line in which they occur (the

macro values in Current Commands will not change). The J code is for part length plus cut-off, so to feed 2.0 inches of bar stock would require the line G105 J2.0.
      Sincerely,
      Haas Applications

• • •

Engraving with Macros (reprise)

(Winter ’04
vol 8 # 28)

  

Dear Applications:

    I want to use the G47 (Text Engraving) command for two different jobs. I’m having trouble getting the text placed exactly where I want it. On  the first one, the specified start position is X0 Y0, but there is an X axis move before engraving takes place. The first character is an M, and the first line it does is an X0.2197 move. Why is this? On the other job I need to center the engraved text on the workpiece. What’s the best way to do that? Thanks.

    Lee Ward

Dear Lee:

    Graphics mode and the single-block function are very useful for engraving jobs. Be sure that Settings 74 and 75 are both turned on.
    The macro program for engraving allows a small amount of space before and after each character. The X0.2197 move occurs when the default size characters (1.0" tall) are being engraved. If you use a J value in the G47 line to change the size, you’ll find that the spacing between characters is reduced or enlarged in proportion to the text size. To start the characters exactly at X0 Y0, run the program in Graphics to see what the first space allowed for the character size is, then program a negative X value in the G47 line. This will compensate for the initial spacing.
    For the centered engraving, again, run the program in Graphics mode and in single-block. Start in the X0 position (on the G47 line) in your work offset. Take note of the work coordinate readings when the last character of your engraving has been completed. That gives you the exact length of the engraving. Subtract this from the width of your part, divide by two, and the result is your starting point on the X axis for perfect centering. Enter this X axis value in the G47 line. This will work with any size font.

    Sincerely,
    Haas Applications

 

Engraving with Macros

(Fall ’03
vol 7 # 27)

  

Dear Applications:

I’ve been using G47 (Text Engraving) for sequential serial number engraving on my VF-4. What causes the machine to increase the number by 1? Is it the M30 at the end of the program? I ran 50 pieces several months ago and numbered them 1-50, and now I want to run another 50 pieces and start numbering them at 51. How do I do this? Do I need to change Macro #599
to 51?
            Curt Olsen

Dear Curt:

The G47 cycle itself is what triggers the counter; after each engraving operation, the counter (macro #599) advances.

You are absolutely correct about setting Macro Variable 599 (in Current Commands) to the serial number you want to start with. The other option you have is to program the initial serial number: In MDI, enter G47 P1(51) to start at SN 51. The engraving section in the operator’s manual has more details about this function.

            Sincerely,
            Haas Applications

• • •

SL-30 Tailstock

(Fall ’03
vol 7 # 27)

  

Dear Applications:

We’re using the tailstock on our SL-30 lathe for the first time. We can’t get the tailstock to hold the part tight – it keeps backing off. It stays tight for about 1 minute or less. We’ve been using the soft key JOG button to move it. Is this the right way to do it? If we try to use the foot pedal, it alarms. What are we doing wrong? Any help on how to use the tailstock would be great.

            Bryan Marshall

Dear Bryan,

The best way to use the tailstock in automatic operation is with the M21 (Tailstock Advance) and M22 (Tailstock Retract) commands. Also, Setting 107 (TS Hold Point) is crucial – you’re getting an alarm when you use the foot pedal because there is either a positive value or the wrong value in Setting 107. You’ll need to enter a negative value here that is about 0.500" past the hold point.

To find this value, press HANDLE JOG, then the B button, then HANDLE JOG again. Using the Jog Handle, manually move the B axis (tailstock) toward the workpiece that has already been center drilled. When you make contact with the center-drilled part, go to the POS-MACH display and find the negative number that is associated with the B axis. Subtract 0.500" more for this move into the part, and enter the resulting negative value in Setting 107. This will cause the tailstock to apply constant pressure on your workpiece when you call an M21. You should also use Settings 105 and 106 for tailstock retract/advance distances. Finally, note that the recommended hydraulic operating pressure is above 120 psi (tailstock pressure gauge is on the front of the machine).

The Haas Operator’s Manual has a very good diagram and explanation of how this works. It’s on pages 94-95 of the current (January 2003) version; if you have an older manual, check the table of contents for “Hydraulic Tailstock Settings.”

            Sincerely,
            Haas Applications

• • •

Quick Code & Visual Quick Code

(Summer ’03
vol 7 # 26)

Dear Applications:

We’ve had a Mini Mill for a couple of years, and recently we got two more. The first one had Quick Code as a source program in the list of programs. I was able to make some nice modifications to this file for our own specific shop use. The two newer machines have a different version of Quick Code and also Visual Quick Code. How would I edit the new Quick Code programs in the newer machines if it’s not in the list of programs? Also, I don’t know where to change the settings or parameters to run the version I loaded in the new machines.
     Frank Huszar

Dear Frank:

Check to see if Setting 23, “9xxx Progs Edit Lock,” is on. If it is on, you will not be able to see the Quick Code or Visual Quick Code (VQC) source program files, since they are defined as 9xxx numbers, O09999 and O09997. You will still be able to use Quick Code or VQC, but you won’t be able to select the source program files to edit the menus and program format. If you turn this setting off, these programs should then be visible, so you can create your own custom menus and program formats.

If you decide to edit your Quick Code source file, you should first save the original program under a different program number (or onto a floppy disk) as a back-up. Then go ahead and modify program O09999 for your custom version of Quick Code. Be sure to back up your customized version after it’s created.

For your own version of Visual Quick Code, edit and customize O09997 (after making a back-up copy). Note that when learning to edit the source program files, it’s easier if you start with Quick Code and progress to VQC later.

You can then load your customized Quick Code or VQC source files on any of your Haas machines that are equipped with the Quick Code options.
    Sincerely,
    Haas Applications

• • •

TL-15 B Command

(Spring ’03
vol 7 # 25)

 

Dear Applications:

I have been going through the programming examples for our new TL-15 twin-spindle lathe. Each process has a B-2.0 command. Where does this number come from? Will it be a constant in any program involving the sub-spindle?
     Gerry Bennett

Dear Gerry:

The B-2.0 in the program examples is to position the sub-spindle (the B axis). The B command or “address” is where the sub-spindle will be when you set offsets for the second operation on the workpiece. Part size is what dictates the B-axis starting point, so this number will be a constant in programs for similar-size parts, where you want to start the sub-spindle work at the same point every time. If B were set to 0 in the program, all of the second-op machining would be done at the far end of the machine. Moving the second-op starting point closer to the main spindle (2 inches closer in this example) reduces cycle time by reducing the distance the turret has to move.
     Sincerely,
     Haas Applications

• • •

Increasing Output

(Summer ’02)
vol 6 # 22)

Dear Applications:

We’re currently making small numbers of a fairly simple part on a three-axis vertical mill. We’d like to increase production to at least 2,000 parts a month, but we’re not sure what kind of equipment and process planning we need. Ditto for a more intricate part: a multi-faced piece that we need to turn out in batches of 20.

     Lynne Little

Dear Lynne:

To increase the production level of your current machine, first look at how many operations each part requires, and then try to consolidate the operations into a single setup. Depending on the size and configuration of the part – and the size of the machine – you may be able to use multiple vises/fixtures, or a rotary table with a multi-sided tooling block, to increase the number of parts machined per load cycle. This will also reduce the number of tool changes considerably (more parts are machined per tool change), and thus shorten your cycle times.

For the multi-faced part, again, you should try to consolidate the operations into the least number of setups. A 4th-axis rotary table will allow you to position the parts for machining on up to four sides in a single setup, which will reduce part handling, cut the number of tool changes and eliminate the tolerance stack-up associated with refixturing.

You should also think about potential bottlenecks in the production flow. Can the part be completed in one setup, or will it require additional work? Establish batch-size and part-transit flow charts that list all of the processes needed to complete the part. Consider part weight and size, the number of parts that can be processed at the same time (including processes such as heat treatment or black oxide) and how many parts can be loaded at a time.

If these jobs will be ongoing, consider investing in a machine designed for higher production, such as a Haas VF-3APCQ Mini FMS with dual automatic pallet changers, or a Haas HS-1RP horizontal machining center with built-in 4th axis and pallet changer. A machine with a 10,000-rpm spindle and programmable coolant nozzle will also speed things up.

     Sincerely,
     Haas Applications

• • •

Pallet Changers

(Spring ’02
vol 6 # 21)

Dear Applications:

I’m running two different parts on my HS-1RP – each pallet has a different part. How can I be sure that the correct program runs on the correct pallet?

     Brandon Hollister

Dear Brandon:

In the Haas pallet-changing machines – both horizontal and vertical mills – it is often useful for the CNC program to test which of two pallets is loaded into the workspace. It has always been possible to do this, but it is not obvious to some users. The following can be used to conditionally execute G-code programs based on which pallet (1 or 2) is loaded into a machine. This can be done even if the user does not have macros.

The code M96 (JUMP IF NO SIGNAL) is used to determine whether a pallet is loaded. M96 allows the G-code program to “jump” to a specific line number (N), based on a test of an input signal to the control. Address codes P and Q are used with M96; P is a subprogram call and Q is the variable being checked (in this case, whether the pallet is loaded).

The following line will cause a jump to N100 if pallet 1 is loaded: 
M96 Q22 P100;

The following line will cause a jump to N200 if pallet 2 is loaded: 
M96 Q23 P200;

If you’re interested, here are the high-tech details. The Diagnostics page is where the control keeps track of which pallet is active. The first bit listed = bit 0; on a horizontal, bit (or input) number 22 is 0 if pallet 1 is loaded, and input number 23 is 0 if pallet 2 is loaded.

Vertical mills may have one or neither pallet loaded. Input number 27 is 0 if pallet 1 is loaded; input number 26 is 0 if pallet 2 is loaded. Both bits will be 1 if neither pallet is loaded. 

On a vertical, the following program line will cause a jump to N100 if pallet 1 is loaded:
M96 Q27 P100;

and the following program line will cause a jump to N200 if pallet 2 is loaded:
M96 Q26 P200;

     Sincerely,
     Haas Applications

 

 

Family-of-Parts Macros

(Summer ’99
vol 3 # 10)

Dear Applications, 

I own a small machine shop with two Haas HL-2 lathes. I manufacture plugs for the medical industry. Many of my products are members of large families (each having the same shape, but with variable dimensions). I don’t want to write a separate program for each part because the control is limited to 200 programs in memory. Is there a way to write a single parametric program for an entire family of parts? Are parametric macro variables compatible with G71?

I have enclosed a drawing of a typical part.

     Sincerely, 
     Jack Hall 

Dear Jack,

Haas recently released an upgrade to lathe control software that allows use of macro variables in G71 and G70 canned cycles. Only one program is required per family. In the example below, the operator simply changes the values for #1 to #6.

 %
 O00001 (G71 G70 PARAMETRIC EXAMPLE) (FANUC COORDINATE) 
#1= 3.25 
#2= 5.45 
#3= 6. 
#4= -1.25 
#5= -1.5 
#6= 0.05 (CORNER BRK + TOOL NOSE RADIUS)
 G20 (INCH)
G00 G54 G40 
G50 S5000 
G96 S1000 M03
T101 M08 
X [ #3 + 0.05 ] Z0.01 
G71 P1 Q2 D0.2 U0.02 W0.005 I0.03 K0.002 
F0.015 
N1 G00 X0 
G01 Z0 F0.005 
X [ #1 - [ #6 * 2 ] ] 
G03 X#1 Z - #6 K - [ #6 ] 
G01 Z [ #4 + #6 ] 
G02 X [ #1 + [ #6 * 2 ] ] Z#4 R#6 
G01 X [ #2 - [ #6 * 2 ] ] 
G03 X#2 Z [ #4 - #6 ] R#6 
G01 Z#5 
G01 X[#3 + 0.1] 
N2 
G70 P1 Q2 
G28
M30 
% 

Sincerely, 
Haas Applications 

• • • • • •

Tool Life Macros

(Summer ’99
vol 3 # 10)

Dear Applications,

I am interested in using a macro statement to test the tool life variables to see if my inserts need to be changed. When the tool can only make one more part, I want to sound a siren to let the operator know he has to attend to the machine and change tooling. 

     Sincerely,
     Carlos Garcia

Dear Carlos, 

Variable #5701 is the tool usage counter, which will accumulate each time Tool #1 is called and used in a program. Variable #5601 is the tool life usage alarm limit that can be set by the operator. The following macro program will accomplish what you want: 

%
 … 
T1 M06 
G103 P1 
(BLANK LINE) 
#1 = #5601 - #5701              (This is setting what you want #1 to represent)
IF[#1 LT 2] GOTO2      (Program will advance to N2 when you have one usage left) 

N1                                                  (Main program) 
G55 G90 G00 X6.215 Y-4. 
G103                                           (Program continues …)
… 
M30

N2 (This sub-routine is going to activate an M function relay that could be wired to a siren) 
IF[#1 LT 2] THEN #1126 = 1  (#1126 is a spare M function in the machine control) 
M00 
M99 P1
 % 

     Sincerely, 
     Haas Applications 

• • •

 

[ Home ] [ MachineCare ] [ Communicate ] [ FeaturesOptions ] [ MiniMachines ] [ MiscTopics ] [ Offsets ] [ Productivity ] [ Programming ] [ Rotary ] [ Thread/Tap ]

 

    

Search CNC Machining On-line!