[GreyFox24]

The company I work for has 2 Hardinge lathes. Both are CHNC styles. I think the other one is a 2 model. Both have 2 different bar feeders. The second machine is down until I get it going. But back to the machine in question. I got the CHNC 1 to run, transfer programs andeverything else they couldn't figure out in the last 10 years here. However,now I am trying to run a bar feed program. (Before it's asked, hand feeding is not a good option as per run time and how small these parts are.) I have asample program to run from our "Experts" that run a big company inseveral locations and it is of no help. The things I see online all say thesame things. So I assume something is wrong with our bar feeder, the machine orflat out we can’t use the bar feeder.

Machine: Hardinge CHNC1
Control Panel: GE Fanuc OT-C
Bar Feeder: Hardinge Bar Feeder (as of now I have no clue on the model number or anything. We have a manual for a HF-4R, but Ithink that is the other bar feeder. Again these are two different models. If Iwas to guess on the serial number, this is a HF-FR6)


The bar feeder is a hydraulic bar feeder. There is a lever to feed, retract, orbe is a neutral state. I have tried leaving it in feed, then tried leaving itin neutral. Same result. I have tried programming this different ways andeverything does the same. We don’t have a direct manual for our machine, but weuse the manual for the Quest models. Our “Experts” tell us it is the samemanual… The sample code says to use M61 for bar feed. The manual says the M61is for “End of Bar Signal.” Which means it should be checking for the end ofthe bar. In which you use a sub program to run the bar feed, but in the mainprogram you use the M61 to tell the machine what to do if it recognizes an endof bar signal. This is another assumption of mine. But when I try using that ortaking it out of the program, I still get this end result:






N*** M21;


(Collet opens, then the programs just hangs indefinitely)





I can’t get it to finish the program, to feed or move the turret, to close the collet, or anything. Of course I have a different view on this situation than the maintenance people, but I want to see if anyone out there has this setup or can help me solve the problem. Any help will be appreciated.





Thank You.

[GreyFox24]

Well I learned that having single block on will cause this to not progress through the program. I get it to open the collet, use my tool to pull back to where I want the bar feeder to stop at, then it closes and errors out immediately. It keeps throwing the alarm for "Collet Delay Not Programmed" of 1004. No matter what I do, I can't get around that. So for a band aide, I have the program set to move to the position I want it to stop to, use a stopper, open the collet and let the bar feeder push the bar into the stop. Then use a M00. So now the operator has to manually close the collet and start it back up. I was trying to avoid the operator having to hit the start button for every part.

[beege]

Good time to give Hardinge support a call. As far as activating /deactivating the bar feeder, IIRC, you press two buttons together, like "SetUp" and "Jog" (I don't remember. been a while). as far as the collet delay think, there should be a G65P9150D1. (or something like that) at the beginning of the program. Someone here will remember each of those...

[GreyFox24]

Thanks for the response. I have seen some sample codes, online, say something like that. Only thing that throws me, is that I am using the bar feed at the end of the program, so does that code need to be at the beginning of the program, or just the beginning of the bar feed portion? Also, the bar feeder we have is "Officially" no longer supported by Hardinge. So I am s.o.l. in that area. Could they be of help? It is possible, but I assume that since they no longer support it, I won't get any help at all. I have seen other quest models use the spindle increase and decrease buttons to activate the bar feeder. Well our bar feeder is directly pneumatic. It's not a hydraulic system like normal people use. So there is no sensors or electrical wiring hooked up to this bar feeder. My only guess is the machine using a solenoid to control air flow to the bar feeder, but the maintenance guys gave me that funny look and proceeded to tell me that wouldn't work. Well it's the only thing we got. I found a work around for my problem, but its not what I wanted to do. I have to baby the operators here so I wanted this as simple as possible. Oh well. I do appreciate the input. I will look into that code for the next program I write for this. I need something consistent beyond what I am using now.

[Machineit]

The collet delay code comes at the beginning of all programs. It is done with an "H" code such as this= H1020 (which is what I use).

I don't use a bar feed, I use a puller. Basically you just need to have the bar-feed ready to feed the bar, bring your stop up to just off of the material, open the collet, back off the bar stop to the desired length, then close the collet again. The collet will close then pause to be sure it is closed tight and then continue you program.

See attached pages from manual.

Mike

[GreyFox24]

Okay. thank you. I will give that a shot. I was doing something like this (this is randomly in the middle of the program):

N600 T0808 S1000 G98
N605 G00 X0.0 Z0.1
N610 G00 Z-0.25
N615 G4 U0.5
N620 M21
N625 G4 U0.5
N630 G01 Z0.05 F100.
N635 G4 U2.0
N640 M22
N645 G4 U0.5


Originally I was getting the collet to open at M21 but then the program wouldn't proceed. Well I learned that single block and M21 don't play well together. Once I turned off the single block, it would actually proceed. Then no matter what dwells it had or if I took them out, the M22, immediately, would error out. Saying the collet delay wasn't programmed. Even though it is clear I put it in there. Not sure if I was using it right, but it was there. So I eventually gave up and bypassed this by this (which isn't how I want this to go in the future):

N600 T0808 S1000 G98
N605 G00 X0.0 Z0.05
N615 G4 U0.5
N620 M21
N625 G4 U2.0
N630 M00
(operator pushed close collet button, then cycle start and machine goes home and ends operation)

In the mean time, I appreciate the help, and the pdf stuff. I got the email and my original question was "What the duece does the number in the H word represent?" But the attachments cleared that up before I had to ask it. The manuals we have, again, aren't directly meant for our machines, but are very loose on help. The sample start up card says to put the H line in there but nothing is said again about it.

H__-__ (collet close command)

(well wtf help is that?) But you cleared that up. Thanks

[Machineit]

I was going to jump in earlier about the single stepping (won't work) but you caught that. I was at home and did not have my manuals with me so replied today.

What controls do you have and do you have manuals? You may have the same Siemens 810T that I have.

Mike

[GreyFox24]

The original post has all the info. I believe the controller is a GE Fanuc OT-C controller. The manuals are all digital. Covers almost everything Fanuc, but what I have. The closest manual is for the quest gt 21 and quest gt 42.

[GreyFox24]

I appreciate the help. Thanks.

[JohnnyTurn]

The collet delay the alarm is referencing is your lack of the 9150 program.
You do not have the collet dwell macro programed at the top of the part program like this:

O5150
G20
G65P9150H2.0
G0T0G30W0
G97 ETC ETC.

Where:
G65 Program call command
P9150: Program 9150 (check your library for this program)
H2.0: Collet dwell time.

When using M21/M22:
The machine will baulk every time without this program called first in your part program.
It's a safety. So the machine will not move until the collet is fully seated. Get it?

G4 Dwells are not the solution.
This method is your solution.

Put the machine back the way it was and try this protocol.
It should work!

This is a standard Hardinge method on CHNC's

JT