plunge with endmill or drill and then plunge

[cuttergrinder]

Last week I had a job at work where I had to drill 8-13/16 holes and put in 2- 1 1/4" flat bottom holes in some 4140. The flat bottom holes are nothing critical, only clearance for a bolt head.

I have been a machinist for over 30 years but this was on manual machines such as cincinnati verticals and g&L horizontal boring mills. On these machines I would put in 1 1/4" flat bottom holes using a 1 1/4" 2 flute high speed endmill and just plunge it right in.

Since we just purchased a Mazak vtc16 cnc mill, I was using this mill and using a 5/8" carbide 4 flute center cutting endmill. I was using the mazatrol and if I remember right, the mazatrol programmed a feed of .008" per rev. I programmed a step down of .150". I backed the feed way down but the machine just did not like plunging with this 5/8 endmill. I ended up drilling the holes to depth with a 13/16 drill and then profiling the holes.

How would you guys go about putting in these flat bottom holes on this machine? What kind of feed would you run and what step down you use?

 

[azmachining]

Not familiar with the machine your using, but from the sounds of it, it lacks power. If it were I, I would try a spiral/radial entry, if it still doesn't like it then I would stick to pre-drilling the holes.

 

[azmachining]

My apologies for not giving you any more info then that, I at the moment am not at the computer with the software to give you the goods.

 

[Hazzert]

Endmills don't like plunging period, you don't notice in aluminum or plastic because they're soft. If you need to plunge I would use a peck drilling cycle at something like a .050 peck and then come back with a pocketing cycle afterwards. I'd also treat the carbide like HSS for speeds and feeds on the pecks, the tool is already doing something it doesn't want to do so why push it?

My preference though would be to ramp or helix down with a 2-3* angle and do it in a couple steps.

 

[G00 Proto]

I set a goal 5 years ago to never ever plunge an end mill. I ramp, pre-drill, circular interpolate, come in from the side (open Pocket)... anything but plunge. I went so far as to set the default plunge rate on all of my end mills to 250 inches per minute. Haven't missed it a bit. Plunging with an EM is unreliable at best. In your case, I would drill the 13/16 hole, then do a high speed circle mill tool path with the 5/8" EM. Rapid down to the bottom of the CB, use some sort of high speed tool path to crank out the material, then a finish path.

 

[SND]

I always drill anything that can be drilled, seems to be the cheapest way to remove metal and saves endmills.

 

[Davis In SC]

I always drill anything that can be drilled, seems to be the cheapest way to remove metal and saves endmills.

+1 Also, a hole plunged with an end mill is Not flat-bottomed... I will admit on rush non critical jobs, I do at times use an endmill as a C'bore, but the surface is dished...

 

[706jim]

I feel vindicated reading this thread. Years ago, I commented that on my 50 taper machine, it didn't seem comfortable plunging with a 1" 2 flute HSS at any more than about 2ipm. The same cutter was fine helical ramping at 30ipm. The comment that I got back then was "I could go faster with a drill press"!
And that plunge was into 6061. Yes, I hate plunging with any end mill; the longer the cutter the worse it seems.

 

[DMF_TomB]

Last week I had a job at work where I had to drill 8-13/16 holes and put in 2- 1 1/4" flat bottom holes in some 4140. The flat bottom holes are nothing critical, only clearance for a bolt head.

I have been a machinist for over 30 years but this was on manual machines such as cincinnati verticals and g&L horizontal boring mills. On these machines I would put in 1 1/4" flat bottom holes using a 1 1/4" 2 flute high speed endmill and just plunge it right in.

Since we just purchased a Mazak vtc16 cnc mill, I was using this mill and using a 5/8" carbide 4 flute center cutting endmill. I was using the mazatrol and if I remember right, the mazatrol programmed a feed of .008" per rev. I programmed a step down of .150". I backed the feed way down but the machine just did not like plunging with this 5/8 endmill. I ended up drilling the holes to depth with a 13/16 drill and then profiling the holes.

How would you guys go about putting in these flat bottom holes on this machine? What kind of feed would you run and what step down you use?

.
.
i believe there is drill cycle for counterbored holes. you drill first then end mill and end mill can be set for width of cut passes. for example at full depth it can take .010 width of cuts circular milling bigger and bigger dia. you can adjust width of cut as much as you want but if 0.200 width of cut at full depth liable to get severe chatter

 

[Bobw]

Plunging sucks... The ONLY time I plunge anymore is when clearing out some softjaws,
and I'm on the Feed Rate pot while its happening, and I still don't like it.

I'm assuming an older Mazak, M32 or M+... That sucks because you can't helix or ramp
without writing a manual process in Mazatrol... I love Mazatrol on a lathe, but
it gets frustrating on a mill if you are doing much more than simple profiling and hole
patterns...

This happened on a Mazak.. I just save it because it looks cool.

 

[DMF_TomB]

Plunging sucks... The ONLY time I plunge anymore is when clearing out some softjaws,
and I'm on the Feed Rate pot while its happening, and I still don't like it.

I'm assuming an older Mazak, M32 or M+... That sucks because you can't helix or ramp
without writing a manual process in Mazatrol... I love Mazatrol on a lathe, but
it gets frustrating on a mill if you are doing much more than simple profiling and hole
patterns...

This happened on a Mazak.. I just save it because it looks cool.

.
.
on mazak i often used manupro (using G and M codes) to have tool stop then go counterclockwise with coolant on to help unwind chips off end mills for a few seconds before tool change. they can buildup a big birds nest of chips fairly quick. i even had M0 at end of manupro to stop cause 10% of time the chip birds nest was still wrapped around end mill. my chips are usually much finer and more numerous than picture

 

[Hazzert]

... This happened on a Mazak.. I just save it because it looks cool.

Coming to Sotheby's 2017?

 

[AndyMoon]

As has been said above - most end mills do not like plunging. The problem is compounded somewhat by the minimal chip clearance on many four flute end mills.

Here is the exception - Guhring "Diver" End Mill - YouTube

Material is 4140 steel. Full disclosure - I work for Guhring and am the product manager for our milling program.

Thanks - Andy

 

[DanielG]

Slight thread hijack, but this thread made me think of a few parts I have coming up. I need to put 1/8" diameter flat bottom holes into aluminum, stainless, and grade 2 Ti. The depth is only .016 to .096 (depending on the hole). My initial plan was to plunge with a 1/8" endmill (different endmills for Aluminum and stainless/Ti obviously), as drilling first wouldn't remove much material at those depths.

An alternative would be to helical interpolate the holes with a 3/32" endmill, but I haven't used anything that small before.

Thoughts?

 

[AndyMoon]

At those depths, a regular end mill shouldn't have too much trouble at slow feed rates. If you have many parts to do, you may want to consider another tool.

As noted above - end mills do not create a true flat bottomed holes. There is a dish on the bottom for axial clearance - so your"flat bottom" will be slightly higher in the middle than towards the OD. In many cases it is not enough to cause an issue for the design intent of the machined component, but it definitely should be considered.

 

[cuttergrinder]

Thanks for the replies guys. I'm sure a helical plunge would be better but I don't think you can do that with mazatrol. I may be wrong since I'm just learning the mazatrol.

 

[plastikdreams]

Thanks for the replies guys. I'm sure a helical plunge would be better but I don't think you can do that with mazatrol. I may be wrong since I'm just learning the mazatrol.

Had to end mill plunge on the Bridgeport Friday, in hardened stavax lol fun times, .3125x.500 deep.

I would much rather a helical interp though.

 

[G00 Proto]

Slight thread hijack, but this thread made me think of a few parts I have coming up. I need to put 1/8" diameter flat bottom holes into aluminum, stainless, and grade 2 Ti. The depth is only .016 to .096 (depending on the hole). My initial plan was to plunge with a 1/8" endmill (different endmills for Aluminum and stainless/Ti obviously), as drilling first wouldn't remove much material at those depths.

An alternative would be to helical interpolate the holes with a 3/32" endmill, but I haven't used anything that small before.

Thoughts?

Helical interpolate with a 3 degree plunge with a 3/16 endmill. Makes a very nice hole. Cutter comp can be tricky because all controls are different on what they require.

 

[G00 Proto]

Thanks for the replies guys. I'm sure a helical plunge would be better but I don't think you can do that with mazatrol. I may be wrong since I'm just learning the mazatrol.

If that is the case, I would still drill first, then plunge down the drilled hole, and do contour passes around the ID of the hole until I got to diameter. You will only be seeing high spindle load when it starts each ID cut.

 

[KilrB]

Helical interpolate with a 3 degree plunge with a 3/16 endmill. Makes a very nice hole. Cutter comp can be tricky because all controls are different on what they require.

You mean 3/32" ... right?

Gonna be hard to make a .125" hole with a .1875" end mill ...