PFH 4800 parameters

We have a PFH 4800 horizontal mill, and it says you can get feeds as high as 2300ipm, It is set now to max at 315ipm, I was told I can put a g61.1 at the start of the program to get more then 315. I would like to set it around 600 - 700, does anyone know what parameter I would have to change, im looking in the book but cant seem to be able to find it

Thanks

Shawn

Don't change any parameters. It's just a G code call out.

After your G43H**Z1., add a G61.1,K70 Now you can feed as fast as you want. Your program should look like this.

G0G90G54X2.Y3.S15000M3
G43H10Z.25
G61.1,K70
G1Z-.25F750.
ETC...
ETC...


The G61.1,K70 will stay active until you enter a G64, or hit reset. You should use it on every tool. It will make all of your corners and chamfers more accurate, even if you're only feeding 100ipm.

Thanks Joe, what does the k70 do?, do you think this is somthing i should add to my post processor, or are there situations where it would not be wanted? I was also told somthing about acceleration issues, that i probally wont hit my disired ipm. do you know anything about this? I found a parameter (M3) this is the feed max. what do you recomend changing?

Ahhh,... High Speed Machining..... Fun stuff...

Ok,...

G61.1,K70: The only thing I would add to your post is the G61.1. You don't need the K70. What K70 controls is the rate of deceleration in the corners. Think of it as a percentage system (and this is a basic description for you). When you go into a tight corner or radius (all controled by parameters), the machine will hit and decelerate in that corner at 70% of the programmed feedrate. So, if you're doing 500ipm, it will decelerate to 350ipm in the corners. If you have a "G61.1,K50", then it will run at 250ipm in the corners and so on. K70 is the machine default and that's why you don't need to set it in the program. But, this is modal (when G61.1 is in use) so if you change (like when you're doing high speed finishing), you'll need to set it back to K70 to return to the default state. Any changes to the "K" value will also return to default at reset, G64 or M30. But if you're flip/flopping between G64 and G61.1 in the same program, the "K" will still remain at what you changed it to until reset, M30 or re-entering the "K70" value.

Now, for the parameters that control HSM,.... Don't change any in the beginning. You don't know what the baselines are or how the machine will react. And each machine is different (even with the same models). 99% of the time, the factory settings for servo gains, vector settings, servo tuning, and etc. are more than sufficient for most. If you're really having problems, that when you might need some tuning. For the most part though, you have plenty of control with the K setting.

I use G61.1 for every tool and therefore it's written into my post. If I need to change it (usually only for finish passes and even that is only "sometimes"), I do it at the time of machine set up.

Of course, all of this doesn't mean much unless your machine has the "2D shape comp" option. Make sure you have it.

thanks man, i decided to leave the machine parameters alone and just use the g61.1, this sounds like the best option to use. we have some high performance endmills comming in i want to test just for the roughing, i probally will keep to the same feeds im running now for finishing. The endmills we are bringing in are suppost to be able to run at a .04 ipt chipload on a 2 flute endmill .400 doc, so at 12000 rpm we should be able to run 960 ipm, to me this sounds way too high, we have a 30hp spindle, I was thinking about maybe cutting this in half to .04 ipr, and a .3doc do you think with this machine i will be able to run these kind of feeds? I run normal 2 flute endmills now at around .01 - .015 ipr with a .3 doc, without any problems

Depends on whose endmills you're using and what diameter. The advantage to High Speed isn't necessarily "how fast and how deep". You'll actually find that you'll get better results with reduced DOC (radial and axial) with high feeds. I've ran 480s at well over 1000 ipm so the speeds are not a problem. Bear in mind, you'll have a bit of a learning curve with part set up, program methods, cutter paths, cutter styles, etc, etc. But man, it'll be fun in the meantime.

Also for note: Even if the cutter could sustain those feedrates and DOC, and the machine could push it, you'll find that the cutter life may shorten too much. Shorter DOC will extend this. Also, KEEP THE COOLANT BLASTING!!!!

Sweet, im looking forward to seeing what this machine will really do, this machine is fairly new to us, we are use to running about 5hp, vtc mills, so this is a big jump for us already, but being anle to get that much more out of the machine will be nice. we also have the high pressure coolant option which may come in handy if we use a collet with thru coolant. Is there a special toolholder you would recomend like a shrink fit, or somthing in those lines, we normally use solid endmill holders, but may try a collet for the thru coolant

Many mill chucks (Lyndex/Nikken, Big Kaiser, etc) have "slots" in them to pass collant. Standard collets (like ER for example) are good as well until you really get into high material removal rates or feeds. The collet flexes too much. I prefer mill chucks (like above) or the CoroGrip from Sandvik. Shrinkers are excelant finishers and can do heavy roughing but you'll need to compensate (for the hollow shank vibrations) the programming a bit in DOC and push the feed more to regain MRR. Also, some tooling (lower quality cutters or improper shank prep) will slip a little in a shrinker so watch that. Doesn't happen often but it can. Also, you can't shrinker a steel shank tool, .... well, you can but you'll never get it out. So Carbide only unless its a tool you don't plan on breaking down.

Solid endmill holders are OK if you use GOOD ones. Like balanced Lyndex or Command and such. They are not my first choice though.

BTW, how "new" is this machine and what control is it?

Thanks for all the input psycho, I find this forum to be very helpful, glad i stumbled across it. The machine will be a year in september and it has a 640m controller 12000 rpm spindle. great machine so far.

Im looking up some new holders now, them things aint cheap. I think we are going to try the lyndex hydraulic chuck, they look like they should work out good, just got to find out whats involved in changing over the cutters

Don't use a hydraulic for milling (except for the Sandvik CoroGrip). Hydraulic chucks are generally intended for precision drilling, reaming, boring and things like that. They are not built to withstand a sideload.

It's also especially worthwhile to get "Pre-Balanced" tooling. They're available off the shelf from most tooling builders. For better pricing you can also look into Techniks, and Tecnara. They are cheaper but still a good quality tool. I just prefer Lyndex/Nikken, Command, Sandvik and Big Kaiser.

With a 12k spindle and a fast control (the 640m), the pre-balanced stuff is worthwhile. It'll increase your tool life, spindle life, accuracy in the machine and repeatability.



Also BTW, most of the tool builders do make pre-balanced, solid end mill holders which will make it cheaper to start up with. But I really can't stress enough about the advantages of the upper end holders.

On the G61.1, we will return to G64 when drilling or tapping. Expecially with G83 or G73 because the machine will feel like it wants to move across the shop floor and it decelerates on every single pecking move. Also when drilling you do seem to take a slight cycle time hit when in G61.1.

PFH4800 excellent machine btw.

Sakis makes a good point. This is an example of where parameter tweeking can adjust alot of this so that the machine doesn't bounce out the back door. You can tune the machines for alot of different reasons to correct difficulties and optimize your process. Also, and I don't know if the machine Sakis is on is, but properly bolting down the machine on a good foundation goes a long way in high speed mode to withstand the accel/decel g-force.

I agree with everything everyone said. Don't use the hydraulic chuck for heavy roughing. Go with a top quality milling chuck balanced to at least G2.5@15,000 rpm, even though you're only going 12,000.

DO NOT run the endmill with a .04ipt and .400 doc. I'm guessing it's an MA Ford Series 135. You'll wear out that poor little 40 taper spindle, and you don't have nearly enough horsepower. Those numbers are meant for 50 taper machines like the Mazak FH8800, and Niigata SPN50 HO.

Run .750 diameter endmill, 12K, .031ipt, .250doc, 75% radial. This will give you 744ipm with a mrr of 116 cubic inches per minute. I don't believe that spindle has all of it's 30 ponies at 12,000rpm, so you should be pretty close to 100% spindle load.

If you're accustomed to 5hp VMCs, this will be more than fast enough to keep you entertained (scared) for quite a while.

If you have a choice between .750 and 1.0 endmills, definitely go with the 1 inch. You'll have to back down those numbers a tiny bit because of horsepower limitations, but it's a better tool.

How large are your parts and how are you fixturing them? If ever there was a chance of a part being thrown from a vise, it's at 750ipm with a .250doc.

Joe, yeah you are right on the endmill, good guess, I dont want to tear the guts out of the machine so i wont be pushing that endmill to its limits, the machine is bolted down so this should help some. Im glad i didnt go and order the hydraulic chucks. these are the holders i am looking at now http://www.lyndexnikken.com/prod_standard.asp?type=milling

The next parts going in there will be aprox 6x4x2 and I will be clamping by aprox .5 in this tombstone http://www.chickworkholding.com/products/system5/multilok4sided.aspx

with profiled jaws.

I dont see any specs on the ultralock system, and we do not curently balance our cutters, but i would think they must be good for at least 12,000rpm.

The Ultra-Locks actually have an inherrent "balanced" condition that runs fairly well and would be a good starting point. I use a lot of the High Speed tooling from them.

Just figured I'd bring this thread back to the top to see if Shawn ever got a chance to put his PFH4800 through it's paces?