question about drilling speed and feed rates

[SpYnOnU]

Hi, I have a couple questions. I'm using a Mori-Seiki mv-80 VMC and I've been drilling these parts they are 1" thick stack drilled (total 2" thick) drilled with a 27.5mm hole. question is I had it running at 500 RPM at 6 IPM and peck at every .4 inches (dont have through spindle cooling) and I've been having a problem with tools burning up as if the speed was too fast but if I turn the speed down a notch to 450 it groans bad going through anybody have any suggestions? and does anybody have a formula I could use? by the way the spade bits are tin coated and there is a spiral flute holder. thanks

[Geof]

What is the material? If they are hot rolled steel or something like that with a scale on it you are subjecting the drill to a double whammy of scale when it is passing through from the top piece into the bottom. It is possible that the heat build up at this point is causing your problem.

You could possibly experiment with your peck distance so that you retract just before reaching the boundary between the two pieces and this will allow coolant in to cool things at the critical point. Possibly even do it in succesive drill cycles; drill down to just reach the boundary in your first cycle then pause for a few seconds with coolant flowing to cool things down before finishing with the second cycle.

[SpYnOnU]

sorry I forgot to mention that, its HR A36 and its been shot blasted so the scale is off for the most part. these parts go onto john deer tractors some frame support and now that you said that I have noticed that it is doing it right as its going into that 2nd piece... so any suggestions I'm still kinda new to programming and haven't experimented too much with the codes but right now I have I.E. (g54g90gox-1.y1.m8, g43h1z1.s500m3, g83 f6. z-2.3 r.1 q.4 p0., so on and so on through the other 5 holes. now isn't the p suppose to be the distance between next peck? is there anyway to have it pull stop for a few seconds then continue? these are fanuc controls I've taught myself everything basically only had a lil help and I've been learning programming on my own, been doing it for about 1 year now. basically I wanna get this to where I can get the fastest cycle time avaliable because generally they will randomly send out an order and want 50 of these parts done within 5 hours when we have a lot of other parts to run. thanks for any replys I appreciate it.

also I will try to get a picture of one of the pieces and a holder to give ya the best idea I can.

[Geof]

I think P is dwell time at the bottom of the hole....which you definitely do not want!!!!

Try my suggestion; drill down to the boundary, retract and pause with a G04 P1000 which should give you 1 second for the cooolant to fill the hole, then start a second drill cycle to go through the bottom piece.

Actually you could do it in three; first one goes to the boundary, then pause, then through the boundary at a reduced speed and feed rate far enough that the drill is cutting full diameter, then a third one at normal feed, pause again and then finish slowly through the bottom.

It is possible that by doing this you can boost you speed and feed in the first and last cycle to save a bit of time and compensate for the dwell and slower feed through the boundary.

The code would be something like this:

M03 S500
G00 Z.5
G83 Z-1. F10. R0.05 Q0.55 (This does two equal pecks)
G04 P1000 (The tool will be at Z.5 giving room for coolant to enter)
M03 S300
{See my comment below}
G00 Z-.95 (Drop down into the hole to save travel)
G83 Z-1.3 F2.5 R-.95 Q0.55 (This does one peck)
M03 S500
G83 Z-2. F10. R-1.25 Q0.55
G04 P1000
M03 S300
G83 Z-2.3 F2.5 R-1.95 Q0.55

{Comment} You would need to have things set Z plane retract above R, I forget the command but during your third drill cycle you want the retract to come clear of the top to get the chips out and let coolant in.

[HuFlungDung]

I don't know about the 'groaning' as the tool goes through, I would not run the drill over 350 rpm, the noise will be whatever the noise will be. The slower speed will cause less coolant throw-off.

If the corners of the tool are already burned off, you'll suffer an intense shriek/squawk as the tool gets further down the hole. Otherwise, the exit should be uneventful, IMO.

I'd probably run about F6. at 350 rpm, so the reduced drill speed does not really cause less throughput than your current production rate.

[dertsap]

i'd say lower speed and use heavy feed ,the bigger drills like to work .
what is the manufacturers recommended sfm for that insert that you are using , normally if you stick within the recommended boundaries the tool should last quite well ,
my concern would be the drill coming down on chips when it re-enters the hole while its pecking , this is normally pretty hard on a tool because the force has to shear thru that chip before it starts to cut .
in my opinion that large of a drill with sufficient flood coolant probably doesn t need a peck cycle

[mhtom]

I've read all the suggestions you got so far and all have good points. I have been using CNC's since they first came out and have not found a peck cycle I liked yet. The deeper you drill the more heat you generate. Heat is a killer. To keep heat to a min. you need to get coolant in the hole. I use my own peck cycle. Three G codes, G00 ( rapid ), G01 ( feed ),G04 ( dwell ). I cut holes in 303 SS from .090 to .5 dia. to a depth of 8.0" deep with no problem. If you need more help contact me and I'll be glad to help you.

[HuFlungDung]

I don't know about Mori, but Haas has a good selection of drill cycles, the G8x series, and the G73 high speed drill cycles. This gives plenty of options for me, and I can get what I need, or if necessary, sequence two different cycles in sequence on the same hole.

[tobyaxis]

Have you tried a High Performance 4 Flute Carbide Drill yet?

If the Spade Drill is all you have then I would try Hu's and Dertsaps suggestions. Bigger Drills like Heavy Feeds and Slow Speeds. I have been told in the past not to Peck with Spade Drills, but to drive straight through uninterrupted. This could be wrong of coarse but I have little experience with Spade Drilling. The places I work are too Old School when it comes to Modern Tooling, LOL.

[SpYnOnU]

thanks for the information guys my lead man is looking into some different tooling after he called and talked to a couple reps from the toolmaker's he had been told the same thing 1.) problem lies with stack drilling and 2.) the feed should be at 6IPM @ 500RPM those are the feeds we had been using, as of friday night the parts were set up once again this time we are running 1 at a time and the machine was groaning even more I changed it to 3IPM at 450RPM so it wouldn't groan as much now we think the problem lies within our fixture as well. all in all its one messed up situation and to the other guy that posted about the place he works being too "old school" yeah our mori was manufactured somewhere between late 80's - mid 90's. so its not the most up-to date piece of equipment and the spindle is another thing thats gonna be looked into however running a 1.5" spade bit through the stack never had a problem I ran it at 300 RPM at 4IPM with no groaning. thanks for any help I appreciate it.