This column is designed to help you and your business perform better. It is a standard feature in CNC Machining. Readers are welcome to submit machining and programming questions to the Haas Applications Department. Haas applications engineers will answer each of your questions promptly, and the best questions will be published with answers in this column.

Dear Applications,

Last month I took delivery of my very first CNC machine, a brand new Haas VF-4 VMC. The control is great! My only problem is that I’ve been unable to get the control to communicate with Hyper Terminal on my PC. I’ve been struggling for weeks with different software settings and cables. H E L P ! ! !

Sincerely,
Dennis Kernighan 

Dear Dennis,

Over the years, Haas CNC machine tools have been successfully interfaced via RS-232 to thousands of computers. However, due to a flood a inquires from customers having difficulties getting Windows-based computers to communicate with a Haas control, now is a good time to set the record straight about using HyperTerminal. 

While HyperTerminal can work, it is very unreliable for this application. In addition, it does not seem to work at all within NT (NT itself is not at fault here). As stated in the Haas Operator’s Manual, general-purpose Windows-based communications programs, like HyperTerminal, will not work reliably with the Haas control. DOS-based programs work much better; however, user resistance to DOS-based programs is growing, and many will not run on NT. 

The solution is to use a Windows-based program written especially for CNC machines. Haas Automation does not provide software; however, we know of several third-party vendors selling a wide range of products which work well with a Haas. Try looking in your monthly trade magazine for a compatible program, or search the Internet for “DNC software.”

One last thing, it is not always necessary to make your own RS-232 cables. Radio Shack stocks excellent cables that work very well. Call the Applications Department (ext. 7342) to obtain correct Radio Shack catalog numbers for your application. 

Sincerely,
Haas Applications

Hyper Terminal is a product of Hilgraeve, Inc. Windows and NT are trademarks of Microsoft, Inc.

Dear Applications,

I own a small job shop with two Haas VF-1 machines. Since I mainly do short runs of any given part, I change setups and work offsets often. I recently nearly crashed my machine because I accidentally called up the wrong work offset. Since then, I always erase any work offsets I am not using to eliminate the chance of calling up the wrong offset and crashing the machine. The problem is that it takes some time to select and erase every individual offset. Is there an easy way to clear all work offsets?

Sincerely,
Brian Channing

Dear Brian,

You could write a simple program using G10 preparatory functions to automatically zero all of your work offsets. It may take a little time to write the program, but it certainly will save time in the future. G10 is usually used to alter offsets within a program, but it also can be used to set offsets to zero. See the programming example below:

Set G52-G59 work offsets to zero:
G10 L2 P0 G90 X0 Y0 Z0 A0 (repeat, changing the value of P, for P0 through P6)
G10 L2 P1 G90 X0 Y0 Z0 A0
 “ “ “ “ “ “ “ “
G10 L2 P6 G90 X0 Y0 Z0 A0

Set G110-G129 work offsets to zero: 
G10 L20 P1 G90 X0 Y0 Z0 A0 (repeat, changing the value of P, for P1 through P20)
G10 L20 P2 G90 X0 Y0 Z0 A0
 “ “ “ “ “ “ “ “ 
G10 L20 P20 G90 X0 Y0 Z0 A0

This could be expanded to set tool offsets to zero by altering the L and P codes. L10-L13 references the geometry and wear columns of length and diameter offsets and P1-P100 reference the tool number offsets. 

Sincerely,
Haas Applications

A Handy Macro
McClain Tool & Technology, Inc., the Haas distributor in St. Louis Missouri, recently sent us this handy macro program which can be used to thread mill just about any size of thread with any size tool. We liked it, so we decided to pass it on to you. 

%
O0001
...
G00 G40 G54 X0 Y0
T1 M06 
S1000 M03
G90 G43 H01 Z0.5 M08
G65 P1234 D1.98 C0.5 E0.0556 Z-0.75 F15. M2
G65 P1234 D2.0 C0.5 E0.0556 Z-0.75 F15. M2 
G00 Z1.
M05
... 
M30

O01234
(MACRO - ID RIGHT HAND STRAIGHT)
(THREAD MILLING WITH MULTI-POINT) 
(TOOL) 
(C=#3 CUTTER DIA)
(D=#7 PASS DIA)
(E=#8 LEAD)
(Z=#26 Z DEPTH)
(M=#13 Z LEAD UP LOOPS) 
G103 P1 (HALT LOOK AHEAD)
(BLANK LINE)
(BLANK LINE) 
IF [#13 EQ #0] THEN #13=1 
G01 Z[#26]F20. (FEED TO BOTTOM) 
#32=[#7-#3]/2 (CALC CUTTER PATH) 
#9=[#9*[#32/[#7/2]]] (CALC FEED RATE CENTER OF CUTTER) 
G03 X#32 I[#32/2]J0 F#9 (APPROACH) 
WHILE [#30 LT #13] DO1
#30 = #30 + 1 
G03 I[-#32]J0 Z[#26+[#8 * #30]]
(THREAD MILL UP)
END1 
G03 X0 I[-#32/2]J0 (ESCAPE) 
G103 (RESUME LOOK AHEAD)
M99
%

If you have a question regarding the operation of your Haas machine or the running of a program (including rotary tables), please fax your request to 805-278-0861, att: Applications, and a Haas applications engineer will follow up and get back to you. If we feel your problem would help others, we will publish it in the following issue of CNC Machining. Or you can send your questions to Haas Automation, 2800 Sturgis Road, Oxnard, CA 93030 • Att: Applications Dept. You can also e-mail your questions to: askhaas@hotmail.com