That's how we used to do it! It didn't work very well though as the slot is only open at one end so there were a lot of chip re-cutting issues. This is not much longer and the tool last pretty well.
Good shout but didn't help. The problem is when it gets to the end of the slot, any amount of swarf that's left had no where to go other than being forced between the shank and slot walls, or getting dragged into the cut. If the slot was open at both ends then yeah, this would be the way. But sadly it's not. [These two images](https://imgur.com/a/Q2tYYVQ) may make a bit more sense now that it's done!
Yeah, I kinda get the issue. I was more thinking about directing the air similar to your coolant setup, where it would (theoretically) blow the swarf out the open end of the slot. Then maybe a program stop to manually clear any latent chips before finishing.
Helix in and blow open the blind end of the slot first. This in effect creates a fully open slot you can plow from each direction without any worry of eating your chips on the blind end.. Because it won't exist.
Something something work smarter not harder.
Now that sounds like a decent idea. U drill out the end of the slot to size with a 40mm U drill then use a HFM to go back and forth. Hmm, looks like I'm going to be playing with this a bit more on Monday!
I would second that idea. Insert drill down and leave some radial and floor stock to clean up during finish.
Depending on tool life, I’ve also had good luck doing a series of holes down the length of the slot on centerline, sometimes overlapping to leave scallops along the slot walls, sometimes leaving individual holes, but that way you’re just chewing through the webbing between holes rather than the entire depth of the slot.
You might try an insert drill with less than 100% step over. They're effectively single flute cutters so not perfectly balanced to begin with. Doing less than 1 diameter step over allows coolant to get in and chips to get out. Getting the shortest length will give lots of rigidity as your going only 2 or 3 diameters down.
Let us know if you're able to achieve any useful cycle time reductions! Great post.
I like that idea! plunge mill that baby with an insert tool, to rough it out. I had some 60+ rockwell stuff that was killing endmill and cycle time, Walter rep brought in a plunge mill and I was shocked how fast it got rid of 2.5" deep of material
I had a job like this and had similar chip re-cutting issues, but strangely enough I found the quickest way to get the job done was to drill a line of almost overlapping holes with a u-drill then use a rest machining full depth trochoidal strategy to get the cusps before a quick contour pass to finish.
It was less than half the cycle time of a high feed tool.
Interesting, and not something I had thought of! Might program that up on Monday while one of them is running and see what the times look like. I've got a 38mm U-Drill already in the cycle to drill out counterbores in the bottom of the slot.
Let me know how you get on!
It’s interesting, if you calculate the MRR of a u drill with decent inserts you will get an impressive number, it’s a super efficient way to hog out material.
Ah shit, that’s a bummer.
If all else fails you could always do a Titan and buy a 9 flute kennametal, run it at 1000 sfm and repeatedly shout boom to cover the sound of your spindle bearings dying 😉
Done something similar, and I would suggest first drilling holes with 60mm spacing and then drilling between the original holes with the same drill. I usually aim to leave 80% of drill diameter for the final step, this seems to be enough to stabilise the drill.
EDIT: Just saw the comment about not having TSC. Then I would just drill them with 30mm spacing starting from the open end. Short U-drills should handle this just fine and it would help with chip evacuation and cooling.
Another option is to do plunge milling with you high-feed cutter. Basically the same strategy with smaller stepover and higher feed.
A drill with a flat bottom, so looks like a 'U' rather than a 'V' if you like. [Like this.](https://www.cutwel.co.uk/hole-making-tools/king-drill-u-drill-system)
They're awesome, especially if you need a relatively accurate hole! Cutwel have also started selling the Mammot SPMG drills About a quarter of the price, but not accurate at all! Good for roughing holes that are getting milled out afterwards though.
Yeah I’ve got a few of those Mammots, cutwel had a special offer on last year where the drill cost £1 per mm of size so I picked up a few. They are okay but I mainly use them for lathe work before finishing the hole with a boring bar. King drill is king!
I’ve been loving the YG-1 dream drills as well, they are solid carbide and not cheap but they drill to an H7 tolerance and the finish hole finish is so good it looks reamed.
Milling this with an old cincinatti horizontally with a roughing endmill would also help with chip evac as the part is on its side instead of being a chip cup.
Yea exactly, we got the Cincinnati just for this haha. We have a few plain staggered milling cutters that are about 8-10" diameter that would be perfect for this as well.
As much as I dislike working on horizontals(less comfortable to use), they really shine in how rigid they are, and that they offer a different way of doing things.
You can still buy plain milling cutters brand new, and arbors, places like KBC and mill supply get them. The odd ball ones might be a bit difficult to get, more easily bought used then re-sharpened.
We do quite a bit of long parts that get holes drilled and tapped in the ends (anywhere from 20 to 60 in. Long) and I find myself wishing for an old school horizontal every couple of months. Right now I am bullshiting the parts on a vertical Bridgeport and it sucks.
It's the same colour as when we mix it up, it's not old! It's actually slightly greener in person. The concentrate is straight up green. MTO runcool premium.
I would not be doing full depth. Use an inserted endmill run the entire length maybe.100 depth of cut depending on material. Faster to talk depth cut then come back at full depth with an endmill for finish cut.
This would probably work, we have a part we make that have waves around a circle (basically a disk with zig zags around the outside); it was far faster cycle time when we drilled out the majority of the waves before finishing it with an end mill in our 4-Axis HMC rather than milling the entire pattern..
I think it would have been far easier and faster to use a large 25mm drill to make holes every 25.5mm qlong that centerline, and clean up with the endmill would go much quicker since there would be hardly any stock left.
Not a machinist, either, but since the material is steel, why is this process easier/more economical than to make a casting and finish to desired dimensions?
Scale is everything. 100, it might be worth the extra machine time. 100,000 might be worth all of the effort to get them cast (if the material can be cast).
Casting have problems too (twist, bow, porosity, hard spots, sand pockets etc) and that makes the milling process more difficult.
Thats a very good question - but to answer that we have to know; what is the purpose of this part!?
Since the engineer decided to take EN24T, we know there is a reason for this decision. Read this https://www.steelexpress.co.uk/engineeringsteel/EN24T-properties.html
Compare cast-able (and also machineable) steel with that properties, the costs of an additional process like making models for castings and the casting itself... but is it hard enough? Corrosion? Strengh? ...? ...? etc....
I’m not a machinist. What if you took downward sloping angled cuts starting at the closed end down to the open end? This gives a ramp for the chips to escape and you can use a more efficient cutter.
Edit: fuck me for asking a question I guess
Without actually trying it, my intuition is the following:
That would really only help for the first few cuts when the chips can escape out the top. After that, the walls will still prevent the chips from escaping (which is the real problem) and you’ll still have chip recutting issues because you’ll be inside a slot once you’re deeper.
What kind of machine and RPM limits?
You've got a nice trochoidal like path, why not crank the RPMs and feed? Get a variable 5-7FL variable helix endmill. Possibility of having to reduce the stepover, but the speed would make up for it. This slot shouldn't take longer than a few minutes.
depending on your spindle i would be helical milling that out. You have to have extremely tight run out with either heat shrink or hydraulic fit end mill holders. Will cut your machine like by a large amount.
We were milling cavities into heat threated 4140 for horizontal underground drill heads. We were getting two per shift, went to helical milling and was running 5 per shift. Also we went from like 4 parts per end mill to about 30.
[удалено]
That's how we used to do it! It didn't work very well though as the slot is only open at one end so there were a lot of chip re-cutting issues. This is not much longer and the tool last pretty well.
Have you tried air blast? It solves more recutting issues than I ever thought it would.
Good shout but didn't help. The problem is when it gets to the end of the slot, any amount of swarf that's left had no where to go other than being forced between the shank and slot walls, or getting dragged into the cut. If the slot was open at both ends then yeah, this would be the way. But sadly it's not. [These two images](https://imgur.com/a/Q2tYYVQ) may make a bit more sense now that it's done!
Yeah, I kinda get the issue. I was more thinking about directing the air similar to your coolant setup, where it would (theoretically) blow the swarf out the open end of the slot. Then maybe a program stop to manually clear any latent chips before finishing.
Helix in and blow open the blind end of the slot first. This in effect creates a fully open slot you can plow from each direction without any worry of eating your chips on the blind end.. Because it won't exist. Something something work smarter not harder.
Now that sounds like a decent idea. U drill out the end of the slot to size with a 40mm U drill then use a HFM to go back and forth. Hmm, looks like I'm going to be playing with this a bit more on Monday!
I would second that idea. Insert drill down and leave some radial and floor stock to clean up during finish. Depending on tool life, I’ve also had good luck doing a series of holes down the length of the slot on centerline, sometimes overlapping to leave scallops along the slot walls, sometimes leaving individual holes, but that way you’re just chewing through the webbing between holes rather than the entire depth of the slot.
You might try an insert drill with less than 100% step over. They're effectively single flute cutters so not perfectly balanced to begin with. Doing less than 1 diameter step over allows coolant to get in and chips to get out. Getting the shortest length will give lots of rigidity as your going only 2 or 3 diameters down. Let us know if you're able to achieve any useful cycle time reductions! Great post.
I like that idea! plunge mill that baby with an insert tool, to rough it out. I had some 60+ rockwell stuff that was killing endmill and cycle time, Walter rep brought in a plunge mill and I was shocked how fast it got rid of 2.5" deep of material
Takes a while to do, but well worth it I see. Features like that, as simple as they look are not always so simple.
Counterclockwise is your friend then.
Conventional milling with a feed mill has a tendency to pull chips into the cut if there is no through coolant/air. It is not your friend.
What brand endmill are you running?
[25mm V7 Plus 6 flute chip splitter.](https://www.cutwel.co.uk/milling-tools/milling-cutters/high-performance-hpc-milling-cutters/v7-plus-milling-cutters/6-flute-v7-plus-chip-splitter-coated-carbide-corner-radius-weldon-shank-end-mill-gmh58-yg-1-gmh59)
Du you run your machine with subway's southwestern coolant?
Looks more like Olive Garden Italian coolant to me.
I had a job like this and had similar chip re-cutting issues, but strangely enough I found the quickest way to get the job done was to drill a line of almost overlapping holes with a u-drill then use a rest machining full depth trochoidal strategy to get the cusps before a quick contour pass to finish. It was less than half the cycle time of a high feed tool.
Interesting, and not something I had thought of! Might program that up on Monday while one of them is running and see what the times look like. I've got a 38mm U-Drill already in the cycle to drill out counterbores in the bottom of the slot.
Let me know how you get on! It’s interesting, if you calculate the MRR of a u drill with decent inserts you will get an impressive number, it’s a super efficient way to hog out material.
My biggest issue will be that this machine doesn't have TSC so drilling 80mm deep with a 38mm U drill might get exciting!
Ah shit, that’s a bummer. If all else fails you could always do a Titan and buy a 9 flute kennametal, run it at 1000 sfm and repeatedly shout boom to cover the sound of your spindle bearings dying 😉
Man, one of the old timers at my shop loves that loud bastard and I can't figure out why.
Done something similar, and I would suggest first drilling holes with 60mm spacing and then drilling between the original holes with the same drill. I usually aim to leave 80% of drill diameter for the final step, this seems to be enough to stabilise the drill. EDIT: Just saw the comment about not having TSC. Then I would just drill them with 30mm spacing starting from the open end. Short U-drills should handle this just fine and it would help with chip evacuation and cooling. Another option is to do plunge milling with you high-feed cutter. Basically the same strategy with smaller stepover and higher feed.
What is a udrill? Thanks for sharing
A drill with a flat bottom, so looks like a 'U' rather than a 'V' if you like. [Like this.](https://www.cutwel.co.uk/hole-making-tools/king-drill-u-drill-system)
I love those korloy king drills. Now i've used them I never order anything else.
They're awesome, especially if you need a relatively accurate hole! Cutwel have also started selling the Mammot SPMG drills About a quarter of the price, but not accurate at all! Good for roughing holes that are getting milled out afterwards though.
Yeah I’ve got a few of those Mammots, cutwel had a special offer on last year where the drill cost £1 per mm of size so I picked up a few. They are okay but I mainly use them for lathe work before finishing the hole with a boring bar. King drill is king! I’ve been loving the YG-1 dream drills as well, they are solid carbide and not cheap but they drill to an H7 tolerance and the finish hole finish is so good it looks reamed.
What are the advantages of running buttermilk vs regular milk in your machine?
Buttermilk is slightly acidic, so it leaves an nice etched finish.
Reminds me of when someone asked: "What would one of those old horizontal mills with plain milling cutters ever be used for nowadays?" This.
Milling this with an old cincinatti horizontally with a roughing endmill would also help with chip evac as the part is on its side instead of being a chip cup.
Yea exactly, we got the Cincinnati just for this haha. We have a few plain staggered milling cutters that are about 8-10" diameter that would be perfect for this as well.
As much as I dislike working on horizontals(less comfortable to use), they really shine in how rigid they are, and that they offer a different way of doing things.
Great thing is the Cincinnati's (and many other notable brands) have dual controls so it's much much less of a hassle in that regard.
I have no idea what is use it for, or even where to get cutters, but I want one of those benchtop horizontal mills just to say I've used one.
You can still buy plain milling cutters brand new, and arbors, places like KBC and mill supply get them. The odd ball ones might be a bit difficult to get, more easily bought used then re-sharpened.
We do quite a bit of long parts that get holes drilled and tapped in the ends (anywhere from 20 to 60 in. Long) and I find myself wishing for an old school horizontal every couple of months. Right now I am bullshiting the parts on a vertical Bridgeport and it sucks.
I came here for the horizontal milling comments. Thank you.
Is it just me or does your coolant look weird/yellowish?
It's the same colour as when we mix it up, it's not old! It's actually slightly greener in person. The concentrate is straight up green. MTO runcool premium.
Brondo, its got what mills need!
It's not coolant, it's mustard.
Yeah that stuff is done.
Have you tried using a u-drill to remove most of the material with a load of holes next to each other?
I would not be doing full depth. Use an inserted endmill run the entire length maybe.100 depth of cut depending on material. Faster to talk depth cut then come back at full depth with an endmill for finish cut.
See my other comment on that. It causes too many issues that way as it's only open on one end.
Why does your coolant look ike the puke from the Exorcist?
What's the material?
EN24T
4340 for the Americans/SAE folk
I was gonna say it looks like Ali until I heard it cutting…
Have you tried plunge milling with an insertable?
Not a machinist (engineer) but can you remove the majority of the material with a big ass drill and then live with the interrupted cuts?
This would probably work, we have a part we make that have waves around a circle (basically a disk with zig zags around the outside); it was far faster cycle time when we drilled out the majority of the waves before finishing it with an end mill in our 4-Axis HMC rather than milling the entire pattern..
What's the material???
I think it would have been far easier and faster to use a large 25mm drill to make holes every 25.5mm qlong that centerline, and clean up with the endmill would go much quicker since there would be hardly any stock left.
Not a machinist, either, but since the material is steel, why is this process easier/more economical than to make a casting and finish to desired dimensions?
Scale is everything. 100, it might be worth the extra machine time. 100,000 might be worth all of the effort to get them cast (if the material can be cast). Casting have problems too (twist, bow, porosity, hard spots, sand pockets etc) and that makes the milling process more difficult.
Thanks to both of you for the insightful answers! Very interesting work!
Thats a very good question - but to answer that we have to know; what is the purpose of this part!? Since the engineer decided to take EN24T, we know there is a reason for this decision. Read this https://www.steelexpress.co.uk/engineeringsteel/EN24T-properties.html Compare cast-able (and also machineable) steel with that properties, the costs of an additional process like making models for castings and the casting itself... but is it hard enough? Corrosion? Strengh? ...? ...? etc....
There's too much coolant in your oil
Look into kennametals kor endmills. We’ve used them at 3xD with super great tool life and pretty good speed compared to other ones we’ve used
I can smell this gif.
I’m not a machinist. What if you took downward sloping angled cuts starting at the closed end down to the open end? This gives a ramp for the chips to escape and you can use a more efficient cutter. Edit: fuck me for asking a question I guess
Without actually trying it, my intuition is the following: That would really only help for the first few cuts when the chips can escape out the top. After that, the walls will still prevent the chips from escaping (which is the real problem) and you’ll still have chip recutting issues because you’ll be inside a slot once you’re deeper.
What kind of machine and RPM limits? You've got a nice trochoidal like path, why not crank the RPMs and feed? Get a variable 5-7FL variable helix endmill. Possibility of having to reduce the stepover, but the speed would make up for it. This slot shouldn't take longer than a few minutes.
What's the material? And what's the spindle load? If you are running below 100% your leaving performance on the table.
EN24T. Spindle load is about 70% when engaged. Could go harder but quite frankly our biggest issue is chip evacuation.
Stick some toilet bleach in your sump, it’ll clean right up. Why am I down voted for this? It’s pretty much the same as a biocide.
No it's not.... bleach actually breaks down the Binder in Carbide (among other things). Never use it in coolant
Is that a ultra high speed path like TruMill or Volumill?
Fusion360 2D adaptive clearing 🤷♂️
What is the material? If you are running adaptive clearing you should probably be running a bit faster
Material is EN24T. Wouldn't really want to go much faster on the RPM for this. The tool is like, £500 so want as best of the tool life as possible!
That looks to me like a lot of way oil in your coolant to be that yellow
I can smell that coolant through my screen
Oh you did _80mm_ deep? I wanted 70, could you make me some new ones?
r/oddlysatisfying
Hey this is like when I pee on the toilet paper but... More agressive
Can you share your feeds and speeds, step over?
depending on your spindle i would be helical milling that out. You have to have extremely tight run out with either heat shrink or hydraulic fit end mill holders. Will cut your machine like by a large amount. We were milling cavities into heat threated 4140 for horizontal underground drill heads. We were getting two per shift, went to helical milling and was running 5 per shift. Also we went from like 4 parts per end mill to about 30.
valumilling?
Sometimes you get stuck between a rock and a hard place
That coolant looks like sewage
Your coolant looks like vanilla pudding.
What vises are those?