Trouble milling a bore

DanielG · Apr 26, 2017

I'm trying to put a 3.625" bore through a 1" piece of mild steel (1018 or A36). The piece is 6"x9" and is held in a Kurt vise on 3/8" parallels, so the workpiece should be solid. I drilled a .625" through hole for entry. As programmed, the bore is roughed by spiraling out with a 1/2" 5-flute Helical coated endmill with 1.25" LOC. The cutter is held in a TG75 collet with 2.75" gage length. The machine is a Trak FHM7 bed mill. Using the manufacturer's most conservative speeds and feeds, I should be running full depth at 3660 rpm (479sfm) and 57.8ipm.

Where I'm having trouble is that no matter how I feed it, it sounds absolutely terrible, with tons of squealing. I was originally using a TG100 toolholder with 4" gage length, but switching to the shorter holder didn't make a difference.

Thanks,
Daniel

SCSA · Apr 26, 2017

What sorr of tool clamping you using? Had guys try and sell me and friends of ours the hydraulic tool holders as very ridgid options. ER32 much better, back to back test. Could also be the tool is too sharp, needs and edge break. Had that before, bastard to cut with no matter what you do.

Sent from my SM-G900I using Tapatalk

DanielG · Apr 26, 2017

SCSA said:
What sorr of tool clamping you using? Had guys try and sell me and friends of ours the hydraulic tool holders as very ridgid options. ER32 much better, back to back test. Could also be the tool is too sharp, needs and edge break. Had that before, bastard to cut with no matter what you do.

It's a TG75 collet. My understanding is that it should be more rigid than an ER collet.

SCSA · Apr 26, 2017

DanielG said:
It's a TG75 collet. My understanding is that it should be more rigid than an ER collet.

Aha.... Well that should eliminate that problem. Cheap Chinese holder? Just asking. I only use China holders for pre-drill in pockets as balance is crap.

Sent from my SM-G900I using Tapatalk

DanielG · Apr 26, 2017

They're older Kennametal holders. I used the same holder/endmill to clean up the ends of the bar stock and it did fine on that straight, outside cut, so I'm not sure what's going on.

sfriedberg · Apr 26, 2017

Consider the cutter rotation and the spiral motion. Are you climb cutting or conventional cutting? Try reversing the direction of spiral motion.

DanielG · Apr 26, 2017

I'm climb milling, but I can try conventional in the morning.

pmack · Apr 26, 2017

What is the width of cut?

DanielG · Apr 26, 2017

Sorry, thought I had that in my first post. .060" (12%)

Finegrain · Apr 26, 2017

If you put a 1/2" endmill in a 5/8" hole and start milling at 12%, the tool will have a far greater actual engagement, due to the 5/8" diameter contour wrapping around the tool. The tool is probably seeing more like 30% early on.

Consider helixing in on a much bigger diameter, like maybe 1-1/4". Then when the tool is at full depth, the 12% will be only a little more than 12% actual engagement.

Regards.

Mike

Orange Vise · Apr 26, 2017

DanielG said:
Sorry, thought I had that in my first post. .060" (12%)

Too high.

Take it down to 0.015" and slowly increase the feedrate if possible.

pmack · Apr 26, 2017

.03 should be about right.

Bobw · Apr 26, 2017

Put it in a set screw holder.. You will instantly remove somewhere around 3 points of movement/chatter.

I know.. A set screw holder doesn't cost as much so it can't be as good.. Put it in a setscrew holder
and see what happens. I bet it sounds a lot better.

DMF_TomB · Apr 27, 2017

DanielG said:
I'm trying to put a 3.625" bore through a 1" piece of mild steel (1018 or A36). The piece is 6"x9" and is held in a Kurt vise on 3/8" parallels, so the workpiece should be solid. I drilled a .625" through hole for entry. As programmed, the bore is roughed by spiraling out with a 1/2" 5-flute Helical coated endmill with 1.25" LOC. The cutter is held in a TG75 collet with 2.75" gage length. The machine is a Trak FHM7 bed mill. Using the manufacturer's most conservative speeds and feeds, I should be running full depth at 3660 rpm (479sfm) and 57.8ipm.

Where I'm having trouble is that no matter how I feed it, it sounds absolutely terrible, with tons of squealing. I was originally using a TG100 toolholder with 4" gage length, but switching to the shorter holder didn't make a difference.

Thanks,
Daniel

.
.
1018 steel with 1/2 end mill and maybe 1.5" stick out at 479 sfpm and 57.8 ipm feed at .060 width of cut ? i would never run a end mill that fast of sfpm roughing 1018 steel.
.
the range they give is maximum usually and needs reducing for many factors. i would try slower rpm and feed a lot. also feed if wear based and off center of cutter if I,J is small and actual feed at cutter circumference is faster often 10x faster
.
myself i would make a bigger hole and use a bigger dia end mill at least 1" dia
.
i suggest you record in a excel file what feeds and speeds and depth and width of cuts you find work for the machine and tool holders you are using. as tool gets longer, tool holder gets longer, you approach machine limits, part starts vibrating you will find many times you cannot run at maximum like no where even close to it and get decent tool life. once you find what works you can adjust in small amounts.
.
by the way feeds and speeds are often based on stub length end mill as it gets 2x longer it will deflect 2x2x2 or 8 times more and when 3x longer it will deflect 3x3x3 or 27 times more. longer lengths always need some adjustment in feeds and speeds and depth and width of cuts

thesidetalker · Apr 27, 2017

DMF_TomB said:
.
.
1018 steel with 1/2 end mill and maybe 1.5" stick out at 479 sfpm and 57.8 ipm feed at .060 width of cut ? i would never run a end mill that fast of sfpm roughing 1018 steel.

480 sfm in 1018 steel is "fast"? oooooookay.

Tom, have you ever considered the cost of shop rate vs tools?

In your case, you'd probably run this tool much slower than it can be by several factors. Say you take 4 hours on a job, but your 1/2" endmill is still in good shape afterwards.

I run the same job in 30 minutes or 1 hour, but the endmill is toast when I'm done.

Lets see... cost of a $40-50 endmill or cost of extra 3 hours shop rate. Which case am I ahead?

Sometimes you just need to stop posting and understand not everybody is running a big ass machine the size of a bus. He's just cutting a hole in a small part in a vise. He doesn't need to worry about scrapping a 10 ton casting. Your experience isn't relevant at all to his situation.

G00 Proto · Apr 27, 2017

I don't run mountains of steel like a lot of the guys on here do, but it seems like your feed is way high for that depth and width of cut for that machine. A bit depends on your tolerance for noise. I used to have a much higher tolerance for loud aggressive cuts, when someone else was buying endmills and repairing "my" machines. If I just had to make a couple of the parts you describe, I would back my feed down by half. If that didn't cure it, I would back my width of cut down by half. Other things that will help would be to use an endmill that has only a 1" LOC. That extra un-used flute is very detrimental to rigidity. I would also use the largest drill in the shop as a pilot drill. Drilling will always be the fastest (common) way to remove material.

I included a picture of your machine from the web as a frame of reference. You don't have the intrinsic rigidity to make deep, heavy cuts using the mfg recommended speeds and feeds. I think that the marketing department usually comes up with those numbers based on the biggest, baddest machine around.

pmack · Apr 27, 2017

I was HSM some 1018 the other day, so I looked at the program. I was running a Guhring 6fl end mill at 6000 rpm, 108ipm, .950 DOC, and .035(7%)stepover. I don't know anything about how rigid a Trak mill is, or if you run high speed tool paths. We have a 5fl Helical running 17-4 H1025 right now at 3600 rpm, 92 ipm, .025 side step, .5 DOC. The helical tools seem to like a lighter radial and more feed.

kenton · Apr 27, 2017

G00 Proto said:
I don't run mountains of steel like a lot of the guys on here do, but it seems like your feed is way high for that depth and width of cut for that machine. A bit depends on your tolerance for noise. I used to have a much higher tolerance for loud aggressive cuts, when someone else was buying endmills and repairing "my" machines. If I just had to make a couple of the parts you describe, I would back my feed down by half. If that didn't cure it, I would back my width of cut down by half. Other things that will help would be to use an endmill that has only a 1" LOC. That extra un-used flute is very detrimental to rigidity. I would also use the largest drill in the shop as a pilot drill. Drilling will always be the fastest (common) way to remove material.

I included a picture of your machine from the web as a frame of reference. You don't have the intrinsic rigidity to make deep, heavy cuts using the mfg recommended speeds and feeds. I think that the marketing department usually comes up with those numbers based on the biggest, baddest machine around.

View attachment 197233

I run a similar southwest mill at work and for a one off part like that I would start at 1100 to 1500 rpm and .0025 feed per tooth with a 10% step over. I would also increase the start hole size or run at 50% feed till the hole was larger.

It took me a long time to accept that these machines just aren't that ridged and often can't take even 1/3 the cut that even a haas vf2 can.

DMF_TomB · Apr 27, 2017

thesidetalker said:
480 sfm in 1018 steel is "fast"? oooooookay.

Tom, have you ever considered the cost of shop rate vs tools?

In your case, you'd probably run this tool much slower than it can be by several factors. Say you take 4 hours on a job, but your 1/2" endmill is still in good shape afterwards.

I run the same job in 30 minutes or 1 hour, but the endmill is toast when I'm done.

Lets see... cost of a $40-50 endmill or cost of extra 3 hours shop rate. Which case am I ahead?

Sometimes you just need to stop posting and understand not everybody is running a big ass machine the size of a bus. He's just cutting a hole in a small part in a vise. He doesn't need to worry about scrapping a 10 ton casting. Your experience isn't relevant at all to his situation.

.
.
he mentioned having excessive noise with his setup. i have often run much slower sfpm and not have had any problems. 1" end mill can be resharpened many times so cost is not a issue. bigger diameter end mill will always be able to take more. more depth and width of cut as well as more ipt often 2x more feed without vibrating. i have literally made many 1000's of small parts of all alloys in a 6" kurt vise. never seen any programmer ever use over 450 sfpm with 1/2 end mill as 1st choice to rough out 1" plate
.
if he is have vibration problems i would suggest a roughing end mill to get most of material out and then finish with a finish end mill. in my experience vibration is much less.
.
i have seen 1.75 dia roughing end mill at 3 ipm seems slow til you realize it can take 1.75 depth, 1.75 width and just plow through in one pass. obviously what ever is used there is hp limits machine and part can take and that might require going slower. if you rough out with roughing end mill dont be surprised if you need 5 to 20 hp thats what happens when you remove 5 to 20 cubic inches per minute. obviously a big carbide rougher can feed much faster but if it needs 20 to 50 hp that might not be practical. a 1" roughing end mill is a more practical size with smaller lower hp machines

BALNH · Apr 27, 2017

It's a proto Trak. Maybe take it in 2 cuts. At 3600 rpm that motor has no balls.

Trouble milling a bore

Stainless

Plastic

Stainless

Plastic

Stainless

Diamond

Stainless

Cast Iron

Stainless

Diamond

Titanium

Cast Iron

Diamond

Diamond

Stainless

Hot Rolled

Cast Iron

Stainless

Diamond

Cast Iron

Similar threads