Tooling advice for 6061.

gundog · Aug 2, 2019

I need to bore a hole 2.5" deep in some 6061 the hole will be centered in a piece of 2.5" square stock hole diameter is 1.91" depth 2.5". I am wondering what type EM to use that would evacuate the chips the best. I have flood coolant. I have never bored anything that deep so I am not sure what to expect. Rougher or just a high helix 2 flute EM? I plan to do a helical tool path. The only thing I have on hand that will go that deep is a 2 flute insert EM but I don't think it will do well getting the chips out so I will buy something else.

Thanks Mike

Illinoyance · Aug 2, 2019

Drill it first. Use the endmill for final size and shape.

You didn't tell us what type of machine you ere running this on. Fortunately this works regardless of machine type.

DavidScott · Aug 2, 2019

How smooth do the side walls need to be? Really the best way to evacuate the chips is lots of coolant. If it is only one I would just use a 1/2" mill with enough LOC to get the job done in a minimum projection tool holder.

wheelieking71 · Aug 2, 2019

The trick here is to use the smallest size tool you can, to hit your nominal dia. in one shot.
This creates the largest void for chips to wash from.
The second trick is to, get as much flood coolant shooting to the bottom of the hole to wash chips up, as you can.
No matter what size tool you attempt to drive down in there, you are going to be relying on the coolant towards the bottom, for chip evacuation. Not the tool.
If the hole goes through? Pre-drill with the biggest drill you can fit down in there, and get the part up in the air so chips can wash out the bottom.
Pre-drill can help in a blind hole as well, but not absolutely necessary. Either way you are going to be regurgitating some chips at the bottom.
It is normal, but you definitely want to minimize it as best you can.
You don't mention what size your 2-fl indexable is, If it is a 1"? that would be ideal.
I tend to like indexables the best for this job. They are almost always more rigid than their fluted counterparts. Short-flute relieved shank would be my second choice.

Vancbiker · Aug 2, 2019

This ^ pretty much says everything I would do.

I used to make a part with a 1.75 thru hole 2" deep. On my first run, I thought I could wash the chips out of the hole well enough. Turned out that I could not wash 100% of the chips out near the bottom and re-cutting chips left an imperfect wall finish. Next run I drilled a clearance hole in the fixture and drilled the part before milling so the chips could flush out the bottom. That took care of the re-cutting.

gundog · Aug 2, 2019

The insert EM I have is this one https://www.glacern.com/em90_2 I have the .625" one. The hole is a blind hole but i could through drill the center portion to wash chips out that would not hurt the part. The piece will be a mount for a crab davit that a 1.5" 6063 schedule 40 pipe will fit in, it will have a cross drilled hole every 90* in the pipe. This part will have a matting hole that is drilled and tapped for a hand knob to index the cross drilled holes in the pipe. The bottom of the 2.5" square stock will have four mounting bolts holding it to another part that mounts to a boat. I plan to make the square stock 3" long overall and bore it 2.5" but a center hole in the bottom would not hurt a thing.

My machine is a Sharp VMC with a 10 HP 10,000 RPM spindle. The flood coolant puts out a pretty good stream out of 2 flex loc hoses and one stream that comes out by the spindle.

wheelieking71 · Aug 3, 2019

gundog said:
The insert EM I have is this one https://www.glacern.com/em90_2 I have the .625" one. The hole is a blind hole but i could through drill the center portion to wash chips out that would not hurt the part. The piece will be a mount for a crab davit that a 1.5" 6063 schedule 40 pipe will fit in, it will have a cross drilled hole every 90* in the pipe. This part will have a matting hole that is drilled and tapped for a hand knob to index the cross drilled holes in the pipe. The bottom of the 2.5" square stock will have four mounting bolts holding it to another part that mounts to a boat. I plan to make the square stock 3" long overall and bore it 2.5" but a center hole in the bottom would not hurt a thing.

My machine is a Sharp VMC with a 10 HP 10,000 RPM spindle. The flood coolant puts out a pretty good stream out of 2 flex loc hoses and one stream that comes out by the spindle.

How many of these do you have to make?

gundog · Aug 3, 2019

wheelieking71 said:
How many of these do you have to make?

I don't know it depends on how they sell 10 to start with. I make products for my own business. I doubt I will need to make large quantities at any one time but I need to make them as quick as possible to keep cost down.

wheelieking71 · Aug 3, 2019

You would do well to get a 1" version of that tool. That way you can punch that hole in one helix.
No drill, no finish tool. Just comp the 1" indexable to get a good fit on the pipe.
The finish from the single tool will be plenty good considering the application.
Max your RMP, feed about 100ipm, and step down about .080-.100/revolution.

wheelieking71 · Aug 3, 2019

Here is a 1.250" indexable punching a 3" hole 2.250" deep after a 1" pre-drill:

It is a right quick way to make a 3" hole. Pretty round, with a decent finish.

gustafson · Aug 3, 2019

I used to do a similar hole until I talked the customer into using extrusion, then ditched them cause they was crazy

I know I used a 3/4 3 flute carbide. did I predrill, hmmm. My tool changer is slow but my machine is fast so I tend to not change tools

i will have to see if I can find that program

A drill is the best way to drill a hole[duh]

IF I already have a drill in the machine I tend to predrill.

Argument against is that the drill point makes the chip load very different at the bottom of the hole where you kind of don't want it. Not a deal killer but you end up either slowing down the whole helical ramp or programming a different piece for the bottom when you ought to be making chips.

Sometimes one gets so tied up thinking about the efficiency of the cutting operation one wastes more time dicking around than it would take to make the part with a cordless drill and a chisel

Wsurfer · Aug 3, 2019

I just did some parts on my new brother- in 6061. 4" square pocket 3.1" deep (through). I used a 3/4" YG-1 3.25 LOC 3 flute end mill using a Maritool stubby side lock holder. helix down every .75" and and HSM spiral out to perimeter. RPM 10000, Step over .07 @ 250 IPM. Worked and sounded really good. The brother can blast some coolant (as long as the tank is full), so chip evacuation was good.

If I didn't have blasting coolant though, I would pre-drill the largest hole I could first.

fmari --MariTool- · Aug 3, 2019

Wsurfer said:
I just did some parts on my new brother- in 6061. 4" square pocket 3.1" deep (through). I used a 3/4" YG-1 3.25 LOC 3 flute end mill using a Maritool stubby side lock holder. helix down every .75" and and HSM spiral out to perimeter. RPM 10000, Step over .07 @ 250 IPM. Worked and sounded really good. The brother can blast some coolant (as long as the tank is full), so chip evacuation was good.

If I didn't have blasting coolant though, I would pre-drill the largest hole I could first.

Wow, thats smoking fast !!

G00 Proto · Aug 3, 2019

How fast do you think he could push a 1 15/16 Insert Drill with his 10 hp spindle. It has literally been a couple decades since I used one and remember them making some amazing chips. If I recall correctly we decorated the shop for Christmas with the chips.

gundog · Aug 15, 2019

I made this part yesterday I used a 1/2" 3 flute EM I drilled a .323" center hole and bored a 1" hole on the bottom 1.5" deep while facing and drilling 4 holes to the bottom needed for this part. The EM was 6" overall and had way too much stick out. I did a helical ramp .100" step down per rev it chattered real bad. I stopped and changed the ramp to .050" per rev and it sounded much better but still not good. I am going to try a different EM with less stick out. The part turned out but I definitely need to approach this differently before running a batch. I plan to send the EM out to have the shank end cut down to minimize the stick out. I used this EM because I got a good deal on it now it will end up costing about the same as getting one that had the right overall length. Thanks for all the suggestions.
Mike

BROTHERFRANK · Aug 15, 2019

What was your feed and speed doing the helical ramp? Did you compensate for the ID tool path? Feedrate should be 50% of what it would be in a straight line. The 50% comes from the ratio of the .5" cutter to the 1" bore. If it was a .75" bore with a .5" end mill, the feedrate should be 1/3 of straight line feed rate for example.

Here is a link to a video that shows a 1/2" end mill helical ramping with no starter hole, .100" per revolution, .875" Dia. bore, 1.25" deep in 6061:

YouTube

That was with one of my favorite 3 flute roughers. Cutter is a large part of the equation.

Wsurfer · Aug 15, 2019

BROTHERFRANK said:
What was your feed and speed doing the helical ramp? Did you compensate for the ID tool path? Feedrate should be 50% of what it would be in a straight line.

Here is a link to a video that shows a 1/2" end mill helical ramping with no starter hole, .100" per revolution, .875" Dia. bore, 1.25" deep in 6061:

YouTube

Awesome !!. I need to step up my ramping angle

wheelieking71 · Aug 17, 2019

BROTHERFRANK said:
What was your feed and speed doing the helical ramp? Did you compensate for the ID tool path? Feedrate should be 50% of what it would be in a straight line. The 50% comes from the ratio of the .5" cutter to the 1" bore. If it was a .75" bore with a .5" end mill, the feedrate should be 1/3 of straight line feed rate for example.

Here is a link to a video that shows a 1/2" end mill helical ramping with no starter hole, .100" per revolution, .875" Dia. bore, 1.25" deep in 6061:

YouTube

That was with one of my favorite 3 flute roughers. Cutter is a large part of the equation.

That is jammin'! So, what rougher is that?

gundog · Aug 17, 2019

BROTHERFRANK said:
What was your feed and speed doing the helical ramp? Did you compensate for the ID tool path? Feedrate should be 50% of what it would be in a straight line. The 50% comes from the ratio of the .5" cutter to the 1" bore. If it was a .75" bore with a .5" end mill, the feedrate should be 1/3 of straight line feed rate for example.

Here is a link to a video that shows a 1/2" end mill helical ramping with no starter hole, .100" per revolution, .875" Dia. bore, 1.25" deep in 6061:

YouTube

That was with one of my favorite 3 flute roughers. Cutter is a large part of the equation.

10,000 RPM 54 IPM chip load .0018 I reduced the chip load because of how much stick out I had. I sent the cutter out to have 1.375" cut off the shank end.

BROTHERFRANK · Aug 17, 2019

wheelieking71 said:
That is jammin'! So, what rougher is that?

That was a Cleveland PM rougher in a side lock. $32 from Rutland back then. They changed their recipe though since for the worse, Hanita PM rougher now is my workhorse in 6061. Can still find those in the 40-50 dollar range.

Tooling advice for 6061.

Hot Rolled

Stainless

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Hot Rolled

Diamond

Diamond

Diamond

Cast Iron

Titanium

Hot Rolled

Hot Rolled

Stainless

Cast Iron

Diamond

Hot Rolled

Stainless

Similar threads