What's new
What's new

Hardinge Conquest 42 SP experience?

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
Thanks Ox! I'm heading over to try this turret zero procedure.

Do you know if the tailstock has a similar homing procedure?



Not sure what a '92 panel looks like (prolly the same) but on a '94 you hold down the ZERO RETURN button down by the E-STOP, and then also hit the TURRET INDEX button above the turret station dial.

It will HOME to pos1. The dial is not functional in this app.


-------------------

Think Snow Eh!
Ox
 

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
I don't think that there is any HOMEING procedure for the hydraulic tailstock/sub-spindle at all.
Only if it is ball-screw driven. And the tailstock wouldn't be ballscrew driven, so I'm gunna say "no".
The LED at home like you said should be all needed.


--------------------

Think Snow Eh!
Ox
 

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
Update on this, I got the tailstock to move by commanding m84 on MDI. the tailstock homing button works once the tailstock has moved toward the spindle. And I bought it. I'll be getting it set up in the next month. I'm looking forward to learning this one. Thank you all for the advice. The more I dug in, the more it looks like a clean, well maintained lathe.
 

nissan300ztt

Hot Rolled
Joined
Jul 26, 2011
Location
Taylor
My shop routinely runs a newer Hardinge Cobra for production jobs. That thing will hold .0002" over several days of running. We did a job a few years back on it, over 15000 brass barrel bushings. Never needed to change an offset once and the customer had a 100% in house inspection. All were within tolerance. That was just a drill, turn, bore thread and part off. 15000 parts took about a week.
 

gcodeguy

Hot Rolled
Joined
Jun 17, 2007
Location
Easton, PA
Bought our first Hardinge Conquest 42 around 1987/1988. Still have it. Holds close tolerance all day on the 316 SS castings it has been set up on for the past approximate 3 years. Also a Conquest 51 from the same time period and a T42. Also a couple newer T42s around 20-25 years old.

Turrets on two had to be rebuilt. Had changed coolant over to water. Went back to oil on those lathes and no problem since.

The SP can be programmed to 5 decimal places. You need to know this when using the G76 threading cycle. It is also based on 5 decimal places so a first pass of Q100 is .001 instead of .01. Only a problem when you copy a program to another lathe and forget to change the P3750 to P375 and the Q1000 to Q100. :)

Is it a tailstock or subspindle? Subspindle maxs at S6000. Limit it to S5000 to avoid broken belts or buy heavier duty belts than what the lathe comes with. On our older lathe, the subspinle uses M84/M85 and uses a switch on the bottom of the subspindle to set how far it moves.

Macro B should be available. On our 2 oldest IF/THEN statements can't be used. Need to make use of GOTO statements. Hardinges come shipped with a deep drill cycle. Oldest used 9135, newer 9136. I like 9136 better and have highly modified ours and use it on all our other Fanuc control lathes.
 
  • Like
Reactions: Ox

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
I hadn't thought about the 5 decimal.place programming details,.especially for functions specified using integers with smallest command unit.
This machine has a tailstock, swe hydraulic bar feeder and chip conveyor. The turret was smooth locking into each position, hope it's solid in use. I'm planning to run it with qualichem 251c to stay compliant with the cleaning/passivation process one of my customers uses.

this has the 16c collet interface built into the spindle which looks great for clearance and z working length. When you run a 3 jaw is therw an off the shelf adapter to couple the chuck drawnut internal thread to the 16c internal thread on the draw tube? Also, is there any drawback to running a kitagawa BB-206 (big bore) vs a B-206? It looks like the big bore would give a bit of extra clearance to sink a part into the chuck, not sure what you give up to get that.

Thanks,
Mike
 

gcodeguy

Hot Rolled
Joined
Jun 17, 2007
Location
Easton, PA
We run most of our lathes with barfeeders. The oldest Hardinge has been set up with a 3-jaw chuck to run castings that are mounted in a round fixture and then the fixture gets placed in the chuck. If I remember correctly it screws directly into the draw tube, but we may have made an adapter to accomplish that. Don't remember.

EDIT: There's not a lot of room between the spindle and tail stock. Mounting a chuck is going to cut into that space. You won't be running long parts. Especially if you need to use a longer drill. I should post a picture of our set up, but haven't done pictures in a long time. The set-up uses a longer drill, and is indexing pretty close to the tailstock.
 
Last edited:

Garwood

Diamond
Joined
Oct 10, 2009
Location
Oregon
The bigger the bore gets for a given chuck diameter, the shorter the base jaws get. The stroke will be the same, you just get less flexibility with jaw/t-nut placement.

A 6" chuck seems like it'd be huge on one of these lathes. I'd get a bigger lathe for chuck work.
 

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
I'm prepping to move this machine in, going to put the chuck on hold until it's installed. As I figure out where to place the machine and bar feeder, I was wondering if anyone had some insight into the bar feeder functionality. The feeder is an SMW Omnibar FS65 and it has a handful of useful sleeve sizes, 1.0", 1.25", 1.625".

The barfeed manual shows the lathe sends a signal to tell the feeder to push and the bar feeder feeds back an end of bar signal. Is the bar feeder pushing the entire time the spindle is turning? It seems like it would need to in order to keep the oil flowing to provide the hydrodynamic bearing support as one pump provide the push force and the bearing flow. From the g code side, I found the codes to open and close the collet. Is there an M code to command the barfeed to push? Does the end of bar signal feed into a macro variable that can be accessed in a program? or trigger some type of stop directly? The bar change process looks pretty straightforward, manual retract, deal with the slug and load a new bar.

The next question is if these machines have any spare M codes and I/O. I don't see anything in the manuals, but haven't dug into the wiring diagrams in depth.

Thanks in advance for any thoughts on this.
Mike
 

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
Is this a 12' bar feeder?

Is this an auto loader as well? (magazine)

No - it won't "push" until it sees a "Collet Open" signal.

Hardinge/Fanuc uses O8997 and O8998 as their barfeeder macro's.

Typically you don't have to doo anything special to make the feder work in cycle.

M21 (main collet open)
G4 X1. (1 sec dwell)
M22 (main collet close)
G4 X1. (1 sec dwell)

At the point in the program that you want it to load a new bar, you would likely put an M61.
I put this at the end of my header - if you will.
I put it just before I call my first tool. (Trigon typically)

So, the control reads the M61 and then looks over at the feeder to see if there is still ample material to run or not. If the feeder says "We're good", it goes on to T101...

If it says "Hey y'all, I'm a bit low on bar ratt now. How 'bout I fetch a new bar eh?"
"OK, but wait 'till I git myself all sitchiated first - K?"

So then it (machine control) will go into O8997 and doo whatever it is that you have in there.
This could be as involved as moving your slides, indexing the turret, or whatnot.
Mine only have M21 (collet open)
Then the machine control signals back "Hey, it's you!"

So it will load a new bar, and then hollars back "It's your problem now!"

Then the main control will go into O8998, which would be refered to as your Top Cut routine.
You are going to close your collet, and perform a cut-off a wee bit ahead of Z0.

I'm not copying this from anything, just making it up as I go, but it's essentially:

M22 (close)
T1212 (Cut-off)
M13 S1000
G0 X1.75 Z.025
G50 S2000
G96 S400
G1 G99 X-.05 F.0035
G0 X2.
T0 X15. Z10. M5
M99

Or sumpthing like that...
But your machine should already have what you need in it.
But you may want to edit the X value in O8998 at each job to save time cutting air.
Otherwise, in the name of safety, just set X slightly bigger than your biggest possible bar and fugetaboutit.

At the end of O8998 Top Cut - it will then drop back into your main program just below your M61 and continue.

At least that's how it is on my 18T and 18iT Hardinge [non-swiss] machines.
IDK how that works on an 0T machine.
Same?
Different?
The only thing that I know is that "0's" suck!


--------------------

Think Snow Eh!
Ox
 
Last edited:

wmpy

Hot Rolled
Joined
Dec 16, 2011
This is a single hydrodynamic bar feeder. It's not a bar loader, so you can ignore everything Ox just wrote. (Sorry Ox!)

Assuming the bar feeder is interfaced to the machine properly... You switch the feeder into Auto mode, and the pump should turn on if the machine has the collet closed and is in Auto mode itself (maybe also MDI). The pump pushes the oil into the tube to support the bar and also to push the bar. So, it's basically always pushing. To do a feed out, you position a stop (could be the side of the cut-off) a short distance in front of the bar, open the collet, move the turret to allow the bar out to the position you want, then close the collet.

In machine Jog mode, the bar feeder pump should not run even if the bar feeder is set to Auto. This is so that you don't accidentally open the collet and have the bar come shooting out.

At the end of the bar, I believe the machine goes into feed hold and a message comes on the screen telling you that the bar has ended. There should also be a light on the feeder that comes on to alert you. You should test this out the first time as the length of the pusher along with how close the bar feeder is to the machine has an effect on the end of bar. Also, the end of bar is sensed by an adjustable pressure switch, so this has to be set properly. Once these things are set the first time, they don't usually need to be messed with. You should just check since it's a new installation for you.

There's also a way to disable/enable the bar feed. You press the E-stop button. Then with it in, you hold the E-stop reset and then press the single block button. Verify this in the manual, as I'm going off memory after a long day. Anyway, with the bar feed enabled, the spindle won't run unless the feeder is in Auto mode. This doesn't work when you want to use it as a chucker. But then with bar feeder disabled, the bar feeder pump won't run at all. So, if you're switching back and forth between running bars and using the machine as a chucker, you'll want to get to know this procedure.

I don't have any experience with extra M codes or inputs. What are you trying to do?

One unique thing about these machines that you need to be aware of is that when using collets, you have to watch out for long tools hitting the headwall. With the collet chuck being built in to the spindle, there is a very short distance between the front of the collet and the headwall. Machines from other builders all use a bolt-on chuck or collet chuck that puts your workholding a good distance from the headwall. I wouldn't be surprised if your machine already has some holes or dents in the sheet metal from where someone ran into this problem. When using a chuck, it's much less of a problem.
 

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
The road to Hell, and all that jazz eh?

I searched the feeder name, but came up snake eyes.


--------------

Think Snow Eh!
Ox
 
Last edited:

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
Thanks for the replies, I could have been more specific knowing it was a single bar hydro feeder. wmpy, that's the functional behavior i understood, thanks for clarifying how it is implemented in the g-code.
The reason I'm asking about M codes is that I'm considering retrofitting an older 6' multi bar iemca feeder I found with a bad control. I want to understand what inputs and outputs the machine can control and how I might be able to integrate the shorter feeder with multi bar capacity.
 

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
What control is it that is dead?

Can you not find a clean / used / one owner replacement on e-bay and just have Iemca program it for you?

The CPU on my first gen LNS Servo likes to go out now and aggin. That is a GE PLC (black Fanuc?) and is a known POS. GE has quit supporting this unit, and so if / when it dies, I fetch a used one and have LNS program it.

They charge X for the CPU back when they could git them, and Y for the programming of it, so if you supplied your own CPU, they were fine with programming it for Y fee. They didn't seem to care. Maybe Iemca would doo the same?

Otherwise, just fetch a working unit. They should be affordable.
BUT - get one with the "servo" ability! Or at least one that does more than jist "push".
The LNS Quick-Load Servo units will monitor every feed, and if you blow a cut-off blade and it doesn't feed out the correct distance, it will put you in ALARM.

This is key to trusting that you can walk away from it.


----------------------

Think Snow Eh!
Ox
 

Mike RzMachine

Cast Iron
Joined
Feb 4, 2007
Location
Utah
Ox,
There was a snafu at iemca during some corporate restructuring ~20 years ago and there are a series of bar feeders that they no longer have the plc program and the plc is obselete, likely the reason this feeder is availabe at scrap cost. I'm leaning away from it as the trays are also expensive/rare. The main limit on the hydraulic is making space (inconvenient but doable), and finding/making feed tubes pistons for smaller stock. It's all a trade off, trying to understand how different feeders work and balancing putting time into a more productive shop layout vs using what I have. It looks like newer bar feeders made big strides with accomodating different bar stock sizes with minimal change over cost, plus the sliding floor mounts, and obviously reliable servo feeders. On the feed failure detection, do you locate a stop/tool on the turret that contacts only if the parting operation failed?

wmpy,
I hadn't thought about the short collet projection and crashing long tools into the wall next to the spindle. In my lucky ignorance a few weeks ago, I grabbed an NOS hardinge qc42 chuck shown below. Somewhere in between collets and a 3 jaw for work clearance. I would need 16c collets anyway and these qc42 style are pretty available surplus. One question for you since you've mentioned swapping between the integrated collet and a 3 jaw. Did you have an adaptor made to thread into the chuck draw nut and reach back to the draw tube with the same external thread as a 16c collet, similar to this QC42 chuck?
1669916910440.png
Thanks,
Mike
 
  • Like
Reactions: Ox

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
Good move on the chuck!
I have a 3" (?) extension/closer on my 51, and I have several holes in my headwall.
I have no clue how you would ever doo anything other than hard turn on a colleted spindle?

Yes, I recommend a decent 4' loader, and with the servo - I feed to my roughing tool, and have been for over 1.5 million parts, and the only time that I would have ever had an insert failure from dooing this is when a large bar might have gotten stuck (a ding, or maybe heavy rust, or ???) and came loose and slammed into the tool. Only happened a handfull of times AFAIK.

This is b/c the servo knows where your part length is, and it is ramping down as it gets there, where the old skewl feeders only know "PUSH". I always feed to a stop. I don't trust it THAT much!

I only really know the LNS feeders, and I would get a Quick Load Servo III. The 1 and 2 have the GE controls, and the 3 is s'posed to have a Mits control that apparently isn't a POS and is not overpriced for service parts. I have no experience on that tho. Not sure if the breaking pendant is an issue on the 3's or not. Black tape holds mine together. Cheap plastic not up to oily machine shop air.

However, I have found the (12ft) Iemca feeder that I am learning currently to be quite heavy duty, and the service folks quite helpful. Even if I have an issue that we have not worked out yet...

So not saying that LNS is the best, just that I have some of those and like them, and know the failures as well.


-------------------

Think Snow Eh!
Ox
 

gcodeguy

Hot Rolled
Joined
Jun 17, 2007
Location
Easton, PA
The first few Hardinge lathes we bought came with their barfeeder. My index position is at the drill X0 position. Open the collet and the bar doesn't get pushed forward. (Can't be in Auto mode to open the collet.)

Then we got an Iemca (12 footer) for another T42. I indexed at the same position. Wanted to push the bar back. Put my finger on the end of the bar and hit the collet button. Just happened that there was a drill in position. I am now missing a chunk of meat by the cuticle. Open the collet on that Iemca and it pushed the bar forward. With only one inch of clearance on the Z-axis, I didn't have much time to get my finger out of the way. Especially since I was used to the other barfeeders and wasn't expecting the bar to try and take my finger off. :(

I can take .09 DOC on the Hardinge lathes in 52100 with 16C collets. (Don't know if they can handle a deeper cut.) On our Daewoo Lynx lathes with 16C collets, I have to take less than .04 DOC if making more than one pass. And this is at F.01 feedrate. Otherwise turning to a shoulder leaves stair steps and a short part as the bar gets pushed back.

Heck, the Lynx can't handle over F.004 with a .500 drill. :( And this is with the pressure set into the red.
 

wmpy

Hot Rolled
Joined
Dec 16, 2011
IMG_0534.jpg
Here you can see 2 of the chucks used on my Hardinges. They both have a drawbar adapter that plugs into where the 16C collet would. I don't remember where we got them. I tried looking on the Hardinge website but was unsuccessful in finding them. It might be worth a call to them. Worst case, you could make your own.
 

wmpy

Hot Rolled
Joined
Dec 16, 2011
The first few Hardinge lathes we bought came with their barfeeder. My index position is at the drill X0 position. Open the collet and the bar doesn't get pushed forward. (Can't be in Auto mode to open the collet.)

Then we got an Iemca (12 footer) for another T42. I indexed at the same position. Wanted to push the bar back. Put my finger on the end of the bar and hit the collet button. Just happened that there was a drill in position. I am now missing a chunk of meat by the cuticle. Open the collet on that Iemca and it pushed the bar forward. With only one inch of clearance on the Z-axis, I didn't have much time to get my finger out of the way. Especially since I was used to the other barfeeders and wasn't expecting the bar to try and take my finger off. :(

I can take .09 DOC on the Hardinge lathes in 52100 with 16C collets. (Don't know if they can handle a deeper cut.) On our Daewoo Lynx lathes with 16C collets, I have to take less than .04 DOC if making more than one pass. And this is at F.01 feedrate. Otherwise turning to a shoulder leaves stair steps and a short part as the bar gets pushed back.

Heck, the Lynx can't handle over F.004 with a .500 drill. :( And this is with the pressure set into the red.
This doesn't seem right. What is the max pressure on the Lynx versus the Hardinges?
 

gcodeguy

Hot Rolled
Joined
Jun 17, 2007
Location
Easton, PA
This doesn't seem right. What is the max pressure on the Lynx versus the Hardinges?
Can look today. I know it is in the green and not at the highest point on the Hardinges. Lynx is in the red at over 400. Three Lynx. All the same problem. These are older lathes.

Also on the Hardinges I can rough face at Z.005, make a turn, rapid back to Z.03 and drop down in X-axis. Do that on the Lynx and you will hit the corner at a rapid move. Need a dwell. Blank line works, but they have a tendency to be deleted. The dwell doesn't. Lynx starts moving on the next block before reaching end point of current block.
 








 
Top