What's new
What's new

Helical Milling Hard A2 Issues

Greyfox97

Plastic
Joined
Jun 17, 2021
I have never had good luck with helical milling (tornado milling) in hard material. I have tried different pitch lengths, new endmills after a few cut (even though the tool looks brand new still), slower, faster. I even tried helical with a pitch and a second helix at the same height with no pitch, then the next move with a pitch followed by a second with no height change. Did that all the way down. I end up with a 1 inch deep hole that tapers about .002". Anyone have any good suggestions on how to fix this? Hard milling holes this way is my enemy. The only thing I cannot figure out for the life of me.
 
Also, I have not. We don't have a high feed that small. We have a 3/8th, (which dont help with this part) but I cuts like crap. The 3/4 is beautiful.
 
One more thing, I have tried different means of machining this. As of now, I am trying to do the pitch, the back to the center, the feed back out and machine a circle at that height. Go back to the center, feed back out, circle with a pitch. Back to the center, feed back out, circle flat. Rinse, lather, repeat. This is the first time trying this. I dont know if it will help. Follow up, the cutter is a 3/16th TiCN ball mill. (Promax premium.)
 
Okay it just deleted my first response. I'm not rewriting all that. Hard A2, 52 hrc. .250" hole for dowel pin. Let me know what else you need to know. I wrote a novel as the first response and now it is gone....
 
Machine? Fixturing? How rigid is the part? What tool are you using? Speeds? Feeds?

Y'know... All the stuff you think about when you're machining a part?
 
It is in a vise. Using 2x4x6 blocks under each side. The sides hang out of the vise. I would say it is a 8 out of 10 for rigidness. I think strap clamps hold way better than a vise. 3/16 TiCN ball mill. S2853, f 5.8, aiming for 140 sfm. It is a monarch vmc75 mill. Cat 50 holder. Short neck with no adapter. Tir was .0002". The hole was .230" before heat treat. Finishes at .250" at 1 inch deep.
 
It is in a vise. Using 2x4x6 blocks under each side. The sides hang out of the vise. I would say it is a 8 out of 10 for rigidness. I think strap clamps hold way better than a vise. 3/16 TiCN ball mill. S2853, f 5.8, aiming for 140 sfm. It is a monarch vmc75 mill. Cat 50 holder. Short neck with no adapter. Tir was .0002". The hole was .230" before heat treat. Finishes at .250" at 1 inch deep.

You're using a ball end mill?
140sfpm might be on the slow side, maybe bump that up to 175-ish. And of course run it DRY. Air blast is fine.
How much in Z are you ramping per revolution?
To ensure minimal taper when ramping, I'd relieve the end mill to only have about 1/8-1/4" of flute. This way the rest of the flute length won't have a say in how straight the hole is.
 
We normally run pre-heat treat at 175 but boss man insist 140 is best. The ball is 3/16 of flute. Relieved 1.2" in length to .008" undersized on diameter. We are running air. The original pitch was .006". I tried .002", .012" and .024". It is hard to explain technique. I have tried 6 different things. From standard, straight tornado down to depth at said pitch variants, to combo of dropping to depth then circling out to diameter after make the circle at a pitch. Im sure im some where in the ball park but i cant seem to find the right ramp angle. Or maybe tornado milling isnt right at all.
 
Also, i meant to add. You questioned the ball endmill. Would you suggest a square corner, or maybe a .005-.01" bullnose? I think the fact that the hole is precut, the ball isnt necessary.
 
I will add that we are making mold components. So i really need the hole to be straight. Not that it matters. I dont think any hole should ever be tapered .002" but this is why im really trying to find a method to hard mill this. We want to stop using the edm for stuff like this. Before i got here, parts spent more time in the edm then any of the milling operations. Thats why he bought the Coromills but never used them until i got here. I appreciate all the help, by the way.
 
How straight is the hole after heat treat before final sizing? Straight enough for a reamer to leave an acceptable hole, or no?
 
I havent checked that. I can. I will say we do not have reamers suited for that. We have basic hss reamers here.
 
How many passes are you taking?

Sounds like you're trying to hit it in one shot. Take a spring pass or two and comp the radius as needed to hit your diameter.

Tools dull quickly in hardened steel. When spring passes are no longer effective in eliminating the taper, the tool is done and needs to be replaced.
 
How many passes are you taking?

Sounds like you're trying to hit it in one shot. Take a spring pass or two and comp the radius as needed to hit your diameter.

Tools dull quickly in hardened steel. When spring passes are no longer effective in eliminating the taper, the tool is done and needs to be replaced.

Well. See. The thing is.... the endmill is probably shot. I have been trying to run the same two holes for 2 days now. I originally had it p4ogrammed to do each hole 3 times in the program. I have done each hole at least 30 times each. None of them got any better. I can open the top up but the bottom wont. So in the future, 175 sfm, relieve shank, and try to do it in one go? (With 2 spring passes) Then stop chasing it if it dont get better? Possibly follow it with the reamer? The hole should be straight after those passes. My boss isnt a fan of new things. Mostly self taught. So he isnt very adveturous. I do think the reamer will end up under the size he wants but that is fixable. He dont want the dowel to come out. If it is .0005" over size, put it in the freezer then install it and it will fit fine.
 
Also, i meant to add. You questioned the ball endmill. Would you suggest a square corner, or maybe a .005-.01" bullnose? I think the fact that the hole is precut, the ball isnt necessary.

I'd most certainly use a bull nose end mill.
What shape is the bottom of the hole? That's why I'm questioning the use of a ballnose.
Is depth tolerance not critical?

If it were me, I'd either try to find a way to ream it, or use a bullnose with about a .02 corner rad.
And if helical cutting isn't working, you could always interpolate it taking depth cuts of about .100" at a time or so.
 
Too bad the hole is there because I would use an MA-Ford Hi-roc drill to start the hole. Then use two endmills to finish the holes. The first endmill would be a bullnose which lasts much longer than a straight edge endmill. Even when you spiral it down it will wear and you will have taper and a worn tip to deal with. Mtndew had a great idea of relieving the endmill which will help quite a bit. Last I may take the finishing endmill and relieve it and cut at full depth if possible.
 








 
Back
Top