What's new
What's new
By:
Advanced search…

Keyseat Cutter help

Rick Finsta

Rick Finsta

Stainless
Joined
Sep 27, 2017
So I've got a job that uses a 0.250" thick, 0.040" double corner radius, 1.75" OD, 1/2" shank (with a small relief due to the depth of the feature) slot mill / keyseat cutter, whatever. 14 tooth, solid carbide. It is cutting 4140 at 41-44HRc. It goes in fine but then hits a cross hole and everything seems to go to hell. I am running it at the manufacturer-recommended speeds and feeds (220SFM or 480RPM)and 0.0005" per tooth feed. Thing is the chips are coming off looking HUGE after it hits that hole. It is like only a few teeth are actually cutting. At least one tooth has now chipped, and it sounds horrible in the cut (I've cut about 24 of these parts and have 8 to go). I have been climb milling but my next thought was switcing to conventional milling and upping to 0.001" per tooth and halving my SFM. Other than the one chipped flute the rest feel sharp but I don't have a microscope. No visible edge wear to the naked eye. I'm holding it in a collet and have checked concentricity. Maybe switch over to a sidelock or borrow/buy a hydraulic?

HELP! This project is way behind schedule and if I break this tool I've gotta get another custom made.
 
Can the cross hole be put in after the undercut? Is the "horrible sound" a harmonic. If so, have you tried "driving" the tool in the cut with the overrides to see if it affects the cutting?

Too late now, but if I was faced with a part detail like what I am envisioning from your description, I'd probably go for 5/32 wide tool and make multiple cuts to get the .25 dimension. If multiple cuts ended up a problem then rough the center out with the 5/32" tool then finish in one pass with the .25 tool.

IMO the 1.75 diameter and .25 face with .04CR is too much tool for a relieved 1/2" shank.
 
Vancbiker said:
IMO the 1.75 diameter and .25 face with .04CR is too much tool for a relieved 1/2" shank.
Click to expand...

This ^^^

Especially in RC40+, there are a dozen ways this combo could get all shaky. The extra-thick chips you mentioned imply that the tool is simply vibrating, with only a couple teeth doing most of the work, hence the chipped tooth. Then, the chipped tooth practically guarantees that the harmonic will get picked up again.

Can you take multiple shallow passes, just to get the tool to survive the final parts? Keep the feed up, just lower the DOC.

Regards.

Mike
 
I would bet that the problem is not where the cutter starts into the interrupted cut but when it
makes contact with the opposite side as the chips are binding on the entry side of the cross hole.

I think roughing using convectional milling with a reduced DOC as you thought... and a finish pass climb cutting for a surface finish...

option 2 would be a linear cut into the cross hole to eliminate the chip issue...
 
You may also have stiffness issues using a collet to hold the part, unless it's in a really good fixture. A typical "Hardinge" style indexing head can move with heavy cuts, compounding the issue.

Maybe break the linear cut into hard-coded line segments, with different F/S to get past the hole and then return to a more optimal settings?

I wouldn't go as high as .001"/T, presumably the cutter has no helix or angle to the teeth? If so, the "bang" as it enters the work is considerable, and that goes up quickly with increased FPT.

Coincidentally, I was using a similar cutter last night (carbide, 3/4 x 3/16 x 1/2" shank) for internal features in some 304 tubing, and was down to 600rpm and .0002"/T to get the life I needed. Short tube held vertically in ~70% engagement soft jaws, so a fairly stiff setup.
 
I need the cross hole in first since it locates the part. I've got about 0.0002" diametric clearance on the pin to the hole (it isn't really a slip fit but it isn't size on size, either). The part is being held by a mitee bite expanding mandrel 26mm in OD. I'm giving it pretty hard on the roughing without issue so it is holding hard, but harmonics could be at play as well. I've played with the feed override but the Okuma has an up/down arrow for spindle override instead of a dial so it is really hard for me to vary in real time with my other hand on the feed knob.

I'll try making several shallower passes - the tool grinder told me to try full depth if possible.

This part is a mirror image of all the others in that I am using the opposite station on the fixture (OP1/OP2) due to locating features and when they are cut away, etc. I didn't seem to have problems until I moved it to this other position, but it has also cut a bunch of parts.

Thanks, guys lots to work with here.

I'm losing my ass on this job and I'm sure this will add another 20min. to each. Yuck.
 
We always conventional cut with keycutters. I would try that first. You say you'll locating off the thru hole, but do you need it to go thru to locate? We've had several jobs where a cross hole created interference, so we would drill it to the depth where it wasn't a problem, run the next operation, and then poke the hole thru on a b/p or with a hand drill.
 
Larry Dickman said:
We always conventional cut with keycutters. I would try that first. You say you'll locating off the thru hole, but do you need it to go thru to locate? We've had several jobs where a cross hole created interference, so we would drill it to the depth where it wasn't a problem, run the next operation, and then poke the hole thru on a b/p or with a hand drill.
Click to expand...
Or if possible make the through-hole through the finished part by .01"? Perhaps cutting the part with a hole in it is harder than a floor with a hole in it?
 
FWIW, if you are doing another run of these take a look at an indexable shell mill style slotter. We have very good success with an Ingersoll 2.5" x .1875" wide tool.

:popcorn:
 
I've got a 0.0002" cylindricity call on the hole, and a 0.002" True Position with another feature... so it has to be there first and everything else gets cut in relation to that and the 26mm mounting hole.

I'm switching to conventional milling and am going to try 0.125" stepovers at 0.005" per tooth? If this doesn't work I'll have to try a thinner slitting saw to rough it maybe. Looks like I was down at 0.0001" per tooth for my first pass (which removes most of the material and goes through the hole, everything else is just cleanup).

One thing that does bother me about Fusion 360 is I don't have the control over linking moves in some toolpaths. It makes it easier to program for most things but means hand edits unless I want this whole toolpath running at 3ipm LOL. I do miss Powermill...
 
Rick Finsta said:
One thing that does bother me about Fusion 360 is I don't have the control over linking moves in some toolpaths. It makes it easier to program for most things but means hand edits unless I want this whole toolpath running at 3ipm LOL. I do miss Powermill...
Click to expand...

I'm not sure what path/strategy you're using in 360, but there is an option to select a linking travel feed (though I don't recall its actual name). It defaults to 39.xxx IPM, maybe tinker with that.

Sent from my SM-G930R4 using Tapatalk
 
Rick Finsta said:
I've got a 0.0002" cylindricity call on the hole, and a 0.002" True Position with another feature... so it has to be there first and everything else gets cut in relation to that and the 26mm mounting hole.

I'm switching to conventional milling and am going to try 0.125" stepovers at 0.005" per tooth? If this doesn't work I'll have to try a thinner slitting saw to rough it maybe. Looks like I was down at 0.0001" per tooth for my first pass (which removes most of the material and goes through the hole, everything else is just cleanup).

One thing that does bother me about Fusion 360 is I don't have the control over linking moves in some toolpaths. It makes it easier to program for most things but means hand edits unless I want this whole toolpath running at 3ipm LOL. I do miss Powermill...
Click to expand...

I don't know if this would help you, (assuming I vaguely understood what you might need.).

Harvey Tool - Carbide Keyseat Cutters - Staggered Tooth - Corner Radius

^^^ staggered keyseat cutter

4 Important Keyseat Cutter Considerations - In The Loupe

.

staggered tooth geometry keyseat cutter.jpg

What the tool geometry can do for you (in some instances) ^^^ (not sure about the hardness of your material though for this tool.).


Some tight tolerances there but kinda understand what you have to reference to.
 
I'm using a Harvey full radius keyseat in another feature and it is AWESOME. Much less challenging cut, though! I did think about staggered geometry, but the tool grinder knew the application and made this...

Incidentally I could literally not go 0.001" bigger on this cutter OD - it already runs into other geometry but luckily that is surfaced away later on.

If I had a 5-axis I'd rough it with a 1/4" High Feed and then finish with the keyseat, and do it before that hole was there! This is a single operation on a 5-axis tabbing it off at the end. *Maybe* it would get refixtured to clean up the tabs.

I'll know in about an hour if the changes worked.
 
Probably not any help, but we had a custom carbide tipped (not solid) made from ABU guys to cut a feature. Aluminum material, so alot different there, but it sounds like crap, BUT cut is good and have not damaged the cutter so.... I dunno, just a thought, even tho you said it had chipped a tooth.... Any way you can step up to 3/4" shank with a necked down area of .5", and try brazed carbide tips to keep cost down? We use a 3/4" side lock to hold this tool, might add some rigidty...
 
Still doesn't sound great but it at least sounds like it is cutting evenly and the chips appear uniform. Here's hoping it'll last another five parts!

Ended up at 0.075" Stepover and 0.0005" per tooth for the first roughing pass. I hand coded the linking moves so they are much faster and honestly the cycle time isn't too much worse.

Thanks for the help, I'll report back if something goes to hell.

ETA I am also conventional milling now.
 
The least amount of fee play in your feed or wobble in your fixtureing will cause the climb milling to grab and chatter...I would definatly try convential milling..agre tha will cause a little more wear to the cutter but likely will not take out teeth.

QT: [I'm holding it in a collet ] may be part of the problem.
 
Hope it finishes the remaining parts. I did not want to conventional mill the insides of the stainless tubes I mentioned in #5 due to risk of work hardening. But if you're getting better cutting now, :cloud9:
 
Could you possibly plunge into the area with the woodruff near the hole first, then cut the slot?
 
You must log in or register to reply here.

Similar threads

R
Help milling slot with tight tolerance
Replies
17
Views
520
camhead420
camhead420
E
Brand name end mill chipped on first light cut?
2 3 4
Replies
62
Views
3K
???
???
M
Cant Break A Chip Help!!
2
Replies
28
Views
1K
triumph406
triumph406
Doozer
Making a shaft from D2 - What to look out for ?
Replies
13
Views
591
Doozer
Doozer
T
Various cutters, 3"
Replies
0
Views
140
Toolchanger
T








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top