Macro's on a 1997 T42 CONQUEST

[Dwayne Foy]

I have a 1997 T42 Conquest Hardinge turning center OT Control . I use Macro's & Var. on my Okuma turning centers but havn't used them on the Hardinge. Is the Macro's on the Hardinge a turn on parameter or will they work now! I bought this machine used in 1998 and have not had Fanuc to turn anything on. Question # two does anyone have a " Deep Drilling Macro" that can but adjusted to drill as program. ( Something like 1st depth 3x dia. , 2nd depth
2-1/2 to 2 x dia. , third depth 1-1/2 to 1 x dia. ...on & on... ).

[g-codeguy]

It is a turn on option. Maybe yours came already enabled. Have you checked yet? The OT control is a bit awkward for Macro B programming. There is no equal or bracket signs on the control panel. Any modification requiring changes using either must be done off-line and the program reloaded.

Also this control does not accept a THEN statement. So far I have been able to find other ways of accomplishing what a simple THEN would do by programming a few extra blocks.

I wrote a simple little macro subroutine that figures depth of cut (plus sets one of two feedrates specified in the macro call based on DOC) that I use in the G71 roughng cycle. This allows me to write one program instead of many for the same part. Can't use it on the OT control. This control will not accept the use of brackets inside the G71. Nor will it allow something as simple as #100=#520+.1093 inside the G71 cycle.

However you can use something like U#500Z-.785 or G1 Z-#500, etc. inside the G71. The OT will accept the use of brackets, etc. as long as it isn't inside the canned cycle.


EDIT. The drill cycle you mentioned sounds interesting, but I don't know of such an animal. However, I feel certain it could be written if you wanted one bad enough.

[cncweblangthang]

at main program

N2(DRILL OPERATION - HSS 1/2 DIA )
G0T0202G97S850M3
G40X0.Z.1T0202
G65P9136K-2.B.02F.01W.5C.2A.5
G0X2.Z2.
T0200
M1

:9136(DEEP DRILL)
IF[#6GE0]GOTO70
G00W0.
#4=#5002
#3=ABS[#3]
#2=ABS[#2]
IF[#19EQ98]GOTO1
#19=99
N1G#19F#9
#27=ABS[#23]
#28=ABS[#6]-ABS[#26]
#29=ABS[#26]
DO1
IF[#27LE#3]GOTO2
GOTO3
N2#27=#3
N3IF[#27GE#28]GOTO4
G00Z[#2-#29]
G1Z-[#29+#27]
G00Z#4
G4U#1
#28=#28-#27
#29=#29+#27
#27=#27*.5
END1
N4G00Z[#2-#29]
G1Z#6F#9
G00Z#4
M99
N70#3000=1(K MUST BE NEGATIVE)

[g-codeguy]

9136 is Hardinge's standard Deep Drill Cycle. It does not do what Dwayne was asking. It cuts the W-value in half, then cuts that value in half, etc., until C-value is reached. The last peck can be any figure less than C-value. Of course, that would be true with the cycle Dwayne is asking for.

[Dwayne Foy]

Cncweblangthang,

Thanks for your reply." Believe it or not" I notice that 9136 is in my program library I have not been able to edit 9136 or is that something that Hardinge has a lock on ? I guess if I use G65P9136K-2.B.02F.01W.5C.2A.5 I don't need to edit macro list. I have been in the machining business sense 1979 and my thoughts are on drilling are 1st entirely 3 to 5 times the dia. 2nd. entirely 3-1/2 to 2-1/2 times the dia. 3rd. entirely 2-1/2 to 1-1/2 the dia. and so on depending on drill type and matl: I have not understood why cnc drilling cycles are not setup that way.
Dwayne Foy

[g-codeguy]

9000 series programs are protected by default when the lathe was purchased. Most people keep the protection turned on. Change parameter 10.4 to 0 if you want to edit the 9136 program.

In your example, P9136 will drill .5 deep, .25, .2 (6 times), and .05 on the last peck. I agree that the program cuts down on peck depths too quickly for many materials. However, in my experience this cycle can be made to work in any material although it may not be the fastest on all occasions because of the depth of the pecks.

I was going to ask if you would like me to try making a macro program that will run the way you have described, but assume you can do it yourself with that much experience. I've only been programming lathes since 1985 which is also when I got into the business. I came from a sheet metal shop before that.

[Dwayne Foy]

G-codeguy,

Thanks for your reply." Yes Go For It " build me a Macro that is adjustable on peck depths. Don't have any experience with Fanuc Macro's and it's rules. We have mostly Okuma equipment expect some horizonal & vertical mills and the one Conquest T42.

Custom Paint Man

[g-codeguy]

I would like to give it a try. Plant is closed until the 4th, so even if I can write it before then, I wouldn't post the program until I had a chance to test it for errors.

In the meantime why don't you try using the 9136 program in the control. These are the variable descriptions for cncweblangthang's example in case you don't have a Hardinge manual.

G40X0.Z.1T0202
G65P9136K-2.B.02F.01W.5C.2A.5

K= final drill depth
B= amount where it rapids to from the previous peck (or from the material for the first peck) before it starts feeding
F= feedrate...natch
W= amount of 1st peck
C= minimum peck (until the last one)
A= dwell at retract position

Not shown in the example is

Z= position where the cycle will start drilling from. Z0 is the default. However, if you previously drilled a bigger hole .375 deep (or was running a casting with a .375 deep counter bore), then this would be your block call:

G65P9136K-2.B.02F.01W.5C.2A.5Z-.375

The drill would rapid to Z-.355 before feeding. Useful.

Not shown or mentioned in any Hardinge manual I've looked at (at least I can't recall seeing any mention of it) is the fact that you can program it for IPM if desired. You can see that from the P9136 program. #19 (S) controls IPM/IPR with IPR being the default. Live tooling is the ONLY time I would select IPM.

SO

G65P9136K-2.B.02F.01W.5C.2A.5S98.

would run the drill in IPM.

Although I agree that cutting the 2nd peck in half from the 1st peck amount is often too much of a cut in pecking depth, I don't believe in running 3x the drill diameter on the 1st peck for all drills or all materials. A .5 inch drill would go 1.5 inches deep before pecking. A standard drill would burn up on the first part in most of the materials we run unless running WAY to slow. YMMV.

EDIT. I can give you an example of how I program the Hardinges if interested. It saves some typing and memory space. It also requires making a couple changes in the parameters. Are the Safe Index subprograms still in your control?

EDIT #2. BTW, just for your own knowledge, I think you will find that you don't have a Conquest T42 but a Conquest 42. I believe Hardinge told me if an OT control is used it is a Conquest 42. If an 18T control is used, it is a T42. Apparently they use those model designations for determining which control is on the lathe. Someone will correct me if my memory is faulty.

[Dwayne Foy]

G-codeguy,

Thanks for your reply. I will try to use G65P9136K-2.B.02F.01W.5C.2A.5 in the mean time. That Z-.375 is a good little code to keep from cutting air.


Custom Paint Man

[g-codeguy]

Mr. Foy, I have your subroutine done tho not tested yet. Before I get into that I wanted to mention another option I thought of while writing your program.

You could slightly modify the existing 9136 program in your control. Replace the W representing the first peck depth with a D representing the drill diameter.

Replace #27=ABS[#23] with #27=ABS[#7]*3 and
Replace #27=#27*.5 with #27=#27*.75

This would drill 3 times the diameter, then 2.25 times diameter, then 1.6875, 1.2656 (rounded), .9492 (rounded), etc. until C (minimum peck) has been reached. Of course you could make the 3 and/or .75 a variable for even more control.

Regarding the program I wrote. First let me mention that it is 2 pages longer than the Hardinge subroutine. That is because their program uses a constant. I used 3x, 2.25x, 1.25x 1x and then .5x for a low limit. These figures basically fall within the mean of the ratios you mentioned in your original post except for .5. I had to set a limit somewhere. Whether or not the program actually will use them all depends on drill diameter, drill depth and the minimum peck specified.

Naturally you could modify any of these values before loading the program....or....consider this. I plan on making a second program by modifying this subroutine. It will require adding 4 more definitions to the G65 call block, but will allow you to individually specify the diameter ratio for the first 4 pecks. Provided, of course, that the hole is deep enough in relation to the drill diameter to use all 4 as a minimum number of pecks.

I will test the subroutine as soon as I can after we go back to work Monday. I'll let you know the results then.

[Dwayne Foy]

G-codeguy

What was the system parameter to be able to edit P9136 ? "Oh By The Way " the reason my logo is Custom Paint Man I have a custom paint and body shop I started 15 years ago. Check out my website eastcoastrefinish.com and see some of my work.

Custom Paint Man

[g-codeguy]

I mentioned it in a previous post, but here it is again. Change parameter 10.4 to 0 if you want to edit the 9136 program. Do you know how to change a parameter on the Hardinge? Just asking. No offense meant. It's easy to ass-u-me too much.

I tested the program on a 21i-T control this morning. Neither of the lathes with an OT control are going to be open for some time. Worked fine. Shouldn't get any different results on an OT.

I will send the program in a PM. Should fit if I don't do a lot of explaining. It drills at the ratios I've already mentioned. Also as previously mentioned, you can change 3 values in the subprogram and add 3 variables to the G65 call to vary the ratios of the first 3 pecks (or all 5 of the first 5 pecks if you want to add 2 more variables).

I will make the modifications and send the modified program in a separate PM. Experiment away. Then let me (and others if they'd like to know) what ratios work the best for you in various materials.

I've tried to allow for all circumstances. From tiny drills to the huge, from brass to the toughest materials.