[g-codeguy]

And I get to be the first to post a thread...if I can type fast enough. How come it took so long to start a Hardinge lathe section? Must be not many people are running these machines.

I like their safe index subprograms, and use them on all the Fanuc controlled lathes I can. I also use their Deep Drill cycle on all Fanuc controlled lathes. Sorry Hardinge! Maybe you don't want me to.

Okay, whose going to be the first to post with a problem on these machines?

[duenow]

And I get to be the first to post a thread...if I can type fast enough. How come it took so long to start a Hardinge lathe section? Must be not many people are running these machines.

I like their safe index subprograms, and use them on all the Fanuc controlled lathes I can. I also use their Deep Drill cycle on all Fanuc controlled lathes. Sorry Hardinge! Maybe you don't want me to.

Okay, whose going to be the first to post with a problem on these machines?

Problem, they last forever. Running my 1992 CHNCI I bought new. still will hold .0002. Also love the safe index & use it on my other fanuc lathes..

[g-codeguy]

Problem, they last forever. Running my 1992 CHNCI I bought new. still will hold .0002. Also love the safe index & use it on my other fanuc lathes..

I started here in 1985. They were running 4 CHNCs at that time. No longer have any. Couple years later the company started replacing them with Conquest 42's. Have one Conquest 51. Still have the 1st 42. Like you said, still running jobs with .0005 total tolerance in materials such as Pyrowear 650.

Only problem we've had lately with this machine is setting work shift. Occasionally it doesn't accept the tool's geometry when you do the MZ. No error message, but you know when it happens as soon as you go to run the first tool.

[DOA]

Problems with Hardinge machines? Come on! lol. I have a Conquest 42, bought it used 5 years ago and had just basic maintenece issues. I have encountered a disater when your in edit mode and the power fails or the machine is shut down. It wipes the system memory clean! You have to reload all the parameters and any part programs. Hradinge Bros walked me thru resetting everything, but after the 3rd time, one of the service techs explained the shutdown problem. Havn't had any trouble since.

[howd]

what is this 'safe index subprograms' you guys are talkin about? I have a Fanuc 18T that I am 'discovering'.

[g-codeguy]

what is this 'safe index subprograms' you guys are talkin about? I have a Fanuc 18T that I am 'discovering'.

Can't do it now, but Monday I can post the programs here if you'd like. Hardinge calls the program O1, O2, O3, O4, O998, & O999. I stuck the first four in 9001-9004 protected programs. Left the last two as listed for the set-up/operators to modify the Z-axis clearance. I could have also put them in a protected program, and used a variable to set the Z with. Trouble is we sometimes have to reverse the X/Z positioning to avoid hitting a subspindle or tail stock. Programs 1, 2 & 999 are used for the main spindle. Others for the subspindle.

Basically these subs cancel G80 series drill/tap cycles, tool compensation, set G0, G97, IPR, etc. 998 & 999 contain the index position. Set-up/operator looks at the longest tool's geometry, and modifies the Z to be an inch (in most cases) longer. Turret will index with one inch clearance from face of part. Provided of course that you use the face as Z0.

Their deep drill cycle is pretty darn good, too. It uses a G65 macro call to set variables for drill depth, distance tool rapids to from the previous cut, feedrate, depth of first pass, minimum DOC (except for the last peck), dwell at retract point, and where the material starts in Z-axis.

If you were running a casting with a counter bore .750 deep, you can program the drills retract point at Z.5, and tell it to start drilling at Z-.75 (minus the tool rapid distance).

So

X0Z.5
G65P9136K-2.265B.02F.008W.65C.25A.2Z-.75

would position drill, set final drill depth at Z-2.265, a rapid clearance of .02, F.008 feedrate, .65 for first peck, .25 minimum peck, .2 second dwell at retract, and start the first drill peck at Z-.73 (.75-.02).

[g-codeguy]

My complete operation for drilling would look like this:

N1000M91 (23/32 HSS DRILL)
T1010S265M13
X0Z.5
G65P9136K-2.265B.02F.008W.65C.25A.2Z-.75
M91
M1

A rough bore would look like this:

N500M91 (ROUGH BORE)
T0505S2500M63
X.747Z.5
Z.03
G1U#510Z-1.96F.01
U-.02
M92
M1

M91 & M92 call up safe index programs 9001 and 9002. Subs are set in M-call parameters. M91 sends tool directly home. First block in M92 is G0Z.5. Therefore it isn't necessary to program a separate clearance move.

These examples are for Hardinge and Daewoos with Fanuc controls.

If I were facing using a G96, I still wouldn't need a G97 in the block where the tool and spindle speed are as it is in the safe index program. I think it makes for a cleaner looking program. Less typing. I'm lazy!

EDIT: I should add that I always start the spindle up with the correct RPM for where I position the tool, then program the G96 block after the approach move. Yes, I am aware that many would simply program a G96 & SFM in the same block with the tool.

[DOA]

what is this 'safe index subprograms' you guys are talkin about? I have a Fanuc 18T that I am 'discovering'.

It is a subroutine program that positions the turret in a preset or defined position in the X and Z axis to allow for indexing without tool to part interference. Look in your manual for Safe start program. It is called by the M98 command. Look up the M98 and M99 code descriptions. You may not have the subprog stored in the buffer either, as well as the subprogs for deep hole drilling.

Sorry for the repeat, lol

[g-codeguy]

what is this 'safe index subprograms' you guys are talkin about? I have a Fanuc 18T that I am 'discovering'.

What machine is this 18T control on?

[TARIQ08]

HI

[torinwalker]

Hello everyone,

Thought I would chime in here and tell everyone that I have a Conquest T42 too. As a matter of fact, I bought it a year ago and have been "restoring" it. Had to take the sub-spindle closer apart and un-freeze it. For whatever reason, the drawtube was seized with rust, shellac, pitting... gawd it was fugly, but I got it all cleaned up and it's working perfectly now. Compared to my old CHNC-1, this thing moves like the devil. Scares the crap out of me when it lurches toward the spindle, even in dry-run mode.

Say, um... does anyone have an example of a sub-spindle to main spindle transfer program? One that actually works? I'm following the example in the programmer's manual on page 16-9, but the G10 P0 Y-n.nnnn command doesn't seem to change the sub-spindle work offset. The sub-spindle moves in absolute coordinates regardless of the work offset programmed. The Z work offset works as expected, but I can't seem to affect the Y offset.

[g-codeguy]

Hello everyone,

Thought I would chime in here and tell everyone that I have a Conquest T42 too. As a matter of fact, I bought it a year ago and have been "restoring" it. Had to take the sub-spindle closer apart and un-freeze it. For whatever reason, the drawtube was seized with rust, shellac, pitting... gawd it was fugly, but I got it all cleaned up and it's working perfectly now. Compared to my old CHNC-1, this thing moves like the devil. Scares the crap out of me when it lurches toward the spindle, even in dry-run mode.

Say, um... does anyone have an example of a sub-spindle to main spindle transfer program? One that actually works? I'm following the example in the programmer's manual on page 16-9, but the G10 P0 Y-n.nnnn command doesn't seem to change the sub-spindle work offset. The sub-spindle moves in absolute coordinates regardless of the work offset programmed. The Z work offset works as expected, but I can't seem to affect the Y offset.

Haven't looked at a manual in years and don't know what you mean by a Y offset. I can check on it tomorrow. The Y-axis is only programmed to pick up the part and eject it. I leave the rapid move to the front of the part and the feed move over the part blank so the setup man can put in the right values. These values are taken directly from the monitor. The Y-axis is sent home after cut-off (G28V0) . There are 3 M-codes pertaining strictly to the Y-axis when it is brought in to pick up the part. Also need the M32 to sync the spindles. Y-axis never moves again until I bring it in a little to eject the part into the part catcher. You set a workshift for the main spindle and another workshift for the subspindle. I use G10P0Z-#530 for the front spindle and G10P0Z-#531 for the subspindle. These values are determined by the setup person. He puts a POSITIVE number in the Macros.

I can send you a sample program tomorrow. Does the lathe have Macro B programming? If not, you can't use my method. If it does, then Hardinge Brothers included a nifty deep drilling cycle with the lathe. It is program 9136. I've improved on it over the years if interested in learning more about it.

[torinwalker]

Since my post, I contacted Bob Allington at Hardinge who look in their manuals, saw the code, and plugged this code into one of their T42's with subspindle. He got the same result! Z is modified, but Y is not. He went to other manuals for similar examples of this usage but could find it nowhere else but in this one T42 manual. So now he thinks G10 P0 Y-x.xxxx is a mistake in the manual. Bob suggested using P10 L2 P1 Yx.xxx instead to achieve the same result (this modifes G54 instead), as one example.

I was just following Hardinge's examples of "best practices" for the most convenient way of doing it. But now that it's wrong, I'm looking for best practices examples for part transfers.

So, yes, please - I'd like to see examples of how you do it.

I learned from here an example of setting safe-start locations using params #500, 501, 502, 503 (safestart X, Y for main, and safestart X, Z for sub, respectively). Having offsets associated by the loaded program and tools (whose locations I also document in my code) is smarter than plugging in G5x offsets manually and trying to remember who set what offset the last time we ran I-don't-know-what-program... With it all in the program, one need only verify tools/collets are where the program says they should be, and go. Your example looks like it follows that same practice, so I'm curious to see your example.

Hmmm... I think my machine does have the Macro B programming - there is an entire interface one follows to create part programs, but I haven't tried it yet. I'll take a look at the drilling cycle. Not sure if the guys who owned this lathe before wiped out or modified those programs (9000-9999) because the inhibit flag is disabled for that block. I'll have a look when I get home from work today.


Torin...

[TARIQ08]

I am trying to thread aluminum tubes on a conquest 42 lathe and i am getting a lot of burrs. I am doing acme thread form, 4tpi. What are the best possible G code

[DOA]

I am trying to thread aluminum tubes on a conquest 42 lathe and i am getting a lot of burrs. I am doing acme thread form, 4tpi. What are the best possible G code

I've not done ACME as big as 4 on my Hardinge, but I have done a bit of 6-8 & 10 tpi's. Your feeds and speeds are very important aa well as the condition and/or style of insert. The best results I got was from using a smaller gauge insert and doing 2 "cycles" with the second pass altered or moved in Z- to widen the profile and minimize the burring. It's virtualy impossible to do the ACME in one "cycle" without burring.

[TARIQ08]

anyone can help me out here, thank you

[groovemixer]

yeah finally!! have to say hardinge is one of top lathes, we have a t42sp about 7 to 8 years old, had some very bad crashes and she still holds to 5 microns!!! trying to purchase another with live tooling this time.

[turnandburn]

Your best bet would be to thread using a g76.

The first G76 block:
G76 Ppppppp Qqqqq Rrrrr

Ppppppp - the first two digits are the number of finish passes, the second two digits are thread pull out chamfer amount, the third two digits are tool nose angle.

Qqqqq - specifies the minimum depth of cut per pass

Rrrrr - specifies amount of stock to leave for the finish pass

The second G76 block:

G76 Xxxxx.xxxx Zzzzz.zzzz Ppppp Qqqqq Rrrrr Fffff

Xxxxx.xxxx - specifies the X end point of the thread.

Zzzzz.zzzz - specifies the Z end point of the thread.

Ppppp - specifies the single depth of the thread.

Qqqqq - specifies the cutting depth of the first pass.

Rrrrr - specifies the taper angle of the thread.

Fffff - specifies the thread lead.

You might want to leave .002-.005 on your od after roughing , then thread, follow with finishing tool to final od, then duplicate your g76 line and give a first pass equal to your single depth and take one spring pass to remove any burr rolled in to threads by your finishing tool.

Hope this helps,

Pete

[g-codeguy]

TARIQ08 , A little more information would be helpful. O.D. or I.D. thread? How are you threading now? RPM, DOC, lead in, etc. I use the G76 thread cycle almost 100% of the time. Do a lot of threading, but it's been years since I did an acme thread. Are you re-turning & re-threading?

[TARIQ08]

I am doing OD threading to aluminum tube 1.32Dia., ID of pipe 0.940, depth .1 and rpm of 900 and using G76 cycle.