Haas Mini Mill Programming Question

[CuttingTools]

What would be the best way to program a series of Identical parts on the same sheet of raw materiaL? what I want to do is machine a series of Flanges ( 40 Pcs total, 8 in the X axis and 5 in the Y axis) on a sheet of 12" x 12" Delrin. These flanges have a 5/8" bore in the center, two mounting holes and an oval shaped outside profile. I have the first flange completely programmed in an absolute mode and with toolcomp on for the outside profile. I put this program into a sub and tried doing a incremental shift ( in abs and Incr mode) to the next piece and then calling up the sub but that will not work as it goes back to the original X,Y Zero location. Any Ideas?

Thanks in advance!

[Rekd]

Are you writing this by hand? Have you tried the quick code?

If you have the NC program for one part, I could transform it to run multiple parts for you with a VB program I made.

[CuttingTools]

Yes I have a verified program for one part. I also have the quick code but I have not found a way to program muliples using the QC.

[Geof]

Originally Posted by CuttingTools What would be the best way to program a series of Identical parts on the same sheet of raw materiaL? what I want to do is machine a series of Flanges ( 40 Pcs total, 8 in the X axis and 5 in the Y axis) on a sheet of 12" x 12" Delrin. These flanges have a 5/8" bore in the center, two mounting holes and an oval shaped outside profile. I have the first flange completely programmed in an absolute mode and with toolcomp on for the outside profile. I put this program into a sub and tried doing a incremental shift ( in abs and Incr mode) to the next piece and then calling up the sub but that will not work as it goes back to the original X,Y Zero location. Any Ideas? Thanks in advance!

G52 would be perfect for this. I would approach this by making the center of the 5/8" bore the work zero for the part and put my machine work zero G54 at the far right corner of the stock.

Relative to the stock dimensions your first part is going to be centered at about X-1. and Y-2. (This is just a rought guess for explanation you will need to accurately locate each center.)

Your default is G54 so you program G52 X-1. Y-1. and then call the sub. Make sure the sub does not mention any work zeroes. The sub uses that G52 location as the work zero for the first part.

Then you program G52 X-3. Y-1. and call the sub again and so on for all the parts.

You will have a program with 40 G52 Xx Yy followed by the sub call and one subroutine.

It does not matter where you have placed the part work zero relative to the part you simply make the X Y in the G52 the place where you want it to be on the stock.

[gar]

060516-1206 EST USA

Cutting Tools:

Forget QuickCode.

You can easily do what you want with G52 in either HAAS or Fanuc mode.

Your program will be in a loop or in a subroutine. At the beginning of each pass (loop or subroutine) you change the values in G52 from within your program.

I have discussed G52 in several different threads. However, the search function in CNCZone is very poor and a search for G52 produces nothing.

I see Geof beat me to a response.

.

[Rekd]

Originally Posted by gar Forget QuickCode. .

I only brought up QC because I wasn't sure if he had it programmed, and if he was using a CAM program.

[Geof]

Originally Posted by gar ......Forget QuickCode.......

Improve efficiency! Don't bother learning QuickCode in the first place

[CuttingTools]

Thanks Geof & Gar for the reply!

I was able to get the first row of parts ( 8 Pcs.) programmed using G10 and incrementing the x axis by 1.375 for each part. After the G10 L2 P1 G91 X 1.375 command I would then call up the sub containing the part geometry. This is a more involved method but it looks like it would have worked. I am going to go back and rewrite the program using your method as it is much cleaner.

Thanks Again for the speedy replies!

[Geof]

Using G10 and incrementing can give you a shorter program in number of lines (I think) but you have to nest your subroutines and have three G10 each in a subroutine. One G10 increments X negative and it is in a subroutine called 7 times another G10 increments Y negative and is called after the 7 calls to the the negative X G10 subroutine and then there is another G10 subroutine which increments X positive called 7 times. Within these subroutines the call to the working subroutine follows each G10 command.

It is certainly a more involved method to initially program but it has the advantage that you can change the positions of your individual work zeroes just by editing two X incremental values and one Y. Also you can extend the array in either direction by changing the L count for the number of times the G10 is incremented. With the G52 method you have to edit all forty G52 commands to change the array and have to add commands to extend the array.

[gar]

060516-1812 EST USA

Cutting Tools:

Go to the following thread and see if you can follow any of the discussion.

http://www.cnczone.com/forums/showth...=g52+haas+mode

Later I will show you how you can increment the G52 values to move from position to position. But fundamentally you need to understand how G52 works in HAAS and Fanuc modes and the differences. G52 can be a very powerful tool.

"michael" "miljnor", if you are viewing this you can protect yourself relative not zeroing G52 by operating in Fanuc mode. But it means whatever values you want in G52 have to be inserted from within your program. Any manually preset values in G52 are zeroed at the start of your program. How is your selector switch working?

.

[gar]

060516-1945 EST USA

A sample using G52. This is the critical portion of a total program.

This illustration is simply for a single axis increment (X), but can be extended to multiple axes. Also this allows you to pre-specify the number of parts to run.

A technique used here for incrementing was required because this must run on our 1993 machine. But this technique illustrates a method that would allow unequal increments, because each position is defined in a table. On a newer machine with equal increments it is much simpler.

Also illustrated in this example is a method to use one tool for all the parts before switching to the next tool.


(Have to use the monkey business of sub 1500 because of HAAS problem.)
(G54 is set to the center of the tooling plate reference hole.)

G52 X 0. Y 0.


(******** You must set value for number of parts ****)

#151 = 1 ( replace 1 with 1 thru 11 for number of repeats wanted. )
( #150 is used for loop counter )

(***********************************)

(Note this capability is very useful to debug a part and then change the count to run multiple parts.)
(This eliminates multiple tool changes at one G52 location, and only does a tool change each N (#151) parts.)



(********************)
(**** TOOL Change to Drill **** --->2 IDD21D HAAS TL # 14 )
( #38 0.101 for self tap screws )

G65 P6901 E54 R 0.101 S 1800 T14 D14 ( call tool chg sub )


#150 = 0 ( initialize loop counter )

N250
M97 P 1500 ( sets G52 for this pass, 150 incremented in N1500 )

G99 G81 F 40.0000 R 0.2000 Z -0.5000 L0
M97 P 16 ( #38 0.101 )

if [#150 LT #151] goto 250

G00 Z 1.5000
G52 X 0. Y 0.
G80





(********************)
(**** TOOL Change to Drill **** --->4 IDD22D HAAS TL # 9 )
( #9 drill )

G65 P6901 E54 R 0.196 S 1800 T09 D09 ( call tool chg sub )

#150 = 0 ( initialize loop counter )

G99 G81 F 40.0000 R 0.2000 Z -0.3750 L0

N251
M97 P 1500 ( sets G52 for this pass, 150 incremented in N1500 )
M97 P 15
if [#150 LT #151] goto 251

G00 Z 1.5000
G52 X 0. Y 0.
G80







(********************)
(**** TOOL Change to Mill Finishing **** -->7 IDM12F HAAS TL # 12 )

G65 P6901 E54 R 0.240 S 5000 T12 D12 ( call tool chg sub )

#150 = 0 ( initialize loop counter )

N252
M97 P 1500 ( sets G52 for this pass, 150 incremented in N1500 )
G0 X 1.0500 Y 1.1225
Z 0.1000
G01 F5.0 M97 P 100 Z 0.1000
G00 G90 Z 0.1000

if [#150 LT #151] goto 252

G00 Z 1.5000
G52 X 0. Y 0.
G80





M09
M05
G90 G0 G53 Z0
G53 X-18.0 Y0
M30






N 1500

( #150 IS INITIALIZED BEFORE CALL TO SUBROUTINE )

IF [ #150 EQ 0 ] GOTO200
IF [ #150 EQ 1 ] GOTO201
IF [ #150 EQ 2 ] GOTO202
IF [ #150 EQ 3 ] GOTO203
IF [ #150 EQ 4 ] GOTO204
IF [ #150 EQ 5 ] GOTO205
IF [ #150 EQ 6 ] GOTO206
IF [ #150 EQ 7 ] GOTO207
IF [ #150 EQ 8 ] GOTO208
IF [ #150 EQ 9 ] GOTO209
IF [ #150 EQ 10 ] GOTO210
IF [ #150 EQ 11 ] GOTO211
#3000= 15 (N1500 - #150 OUT OF RANGE)

N200 G52 X0.
GOTO1501
N201 G52 X-2.1
GOTO1501
N202 G52 X-4.2
GOTO1501
N203 G52 X-6.3
GOTO1501
N204 G52 X-8.4
GOTO1501
N205 G52 X-10.5
GOTO1501
N206 G52 X-12.6
GOTO1501
N207 G52 X-14.7
GOTO1501
N208 G52 X-16.8
GOTO1501
N209 G52 X-18.9
GOTO1501
N210 G52 X-21.
GOTO1501
N211 G52 X-23.1
GOTO1501

N1501
#150= #150 + 1
M99

.

[CuttingTools]

Give me a few days to look over and digest the use of the G52 command. I have managed to get a working program using G10 but I would also like to learn more about G52. After the current job is done on the machine I will have some time to experiment. Thanks again for all your help!