What's new
What's new

Speeds and Feeds for Long Tools

Rcgiovannani

Plastic
Joined
Apr 6, 2015
Hi Guys,

Having a problem and Harvey Tool isn't open today.

I'm running a job in pure aluminum, Series 1000. I'm using Harvey 879308-C8 (DIA 0.125, .187LOC, 1.500RCH, 3FL, - V-Helix with TiB2 coating). It's 12X Reach. Machine is BT30, running Nikken BT30-MMC8C-105-AA holder. Currently the tool is running out about .0001"-.00015" (I only have a tenths indicator, it's running out a little more than a tenth).

I'm getting terrible chatter with the parameters I was given. Here they are:

Roughing (full slot)
RPM - 27K
Axial DOC - .035"
Feed - .0007ipt (56.7ipm)

Finishing
RPM - 27K
Axial DOC - .125"
Radial DOC - .010"
Feed - .00097ipt (78.6ipm)

The feature I'm creating is a 5mm Diameter, flat bottom hole. It's 27mm deep. I am drilling out the center with a 2.26mm Drill before the roughing.
I also tried helically boring the hole with no luck. Also reduced RPM to 15280 (500 sfm), with the same feed per tooth and no luck. I feel like I can never get these long reach tools to cut well... Also played with the feed override a bit - 50-150% and couldn't get rid of the chatter.

I just discovered that Harvey makes a flat bottom drill that will work, but I can't really wait for Tuesday...any help is greatly appreciated!
 

newcomer

Plastic
Joined
Nov 28, 2014
For deep holes, a pilot hole is critical for success. Use a short rigid tool to make a 2xD pilot hole to size. Do not undersize it as your next tool will make her scream as it enters. Approach with your long tool and start at low rpm to enter hole, go full speed and start pecking. If you start at a high rpm with your long tool it'll "whip" and mess up your pilot hole. Do not go full depth in your peck cycle as chip evacuation will likely rear its ugly head. If needed break up the drilling session into a few cycles, and in between shoot your load I mean coolant into the hole to flush out any remaining chips. X Y Z moves may be necessary.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
If it's just a hole (round, no irregular features), why not drill with a modded stub drill, or drill, then follow with a flatted bottom finish drill? Have you never ground a drill bit to change the point angle?

Pure aluminum is very grabby, if you have the option I'd richen the coolant as much as you dare. Make sure the coolant nozzles are well aimed to flush the hole.
 

crossthread82

Cast Iron
Joined
Apr 1, 2022
Location
Maryland
My 12xD harvey chart says you should be running the following (this is for their generic 12xd endmills not the aluminum specific ones):

Slotting:
750SFM (23k rpm)
15% axial (0.01875")
0.00074ipt (51.1ipm)

Finishing:
1000SFM (30.5k rpm)
150% axial (0.1875")
10% radial (0.0125")
0.00176ipt (161.0ipm)

I've helix bored with tools longer than 12xd before, you just have to go really light on the stepdown. In your case probably around .010" then do the suggested speed and feed.

As an aside I've never found Harveytool stuff to cut particularly quite. Especially they're long reach stuff, for longer reach applications in aluminum I like the Destinytool Viper ERS line they have out now.
 
Last edited:

Rcgiovannani

Plastic
Joined
Apr 6, 2015
My 12xD harvey chart says you should be running the following (this is for their generic 12xd endmills not the aluminum specific ones):

Slotting:
750SFM (23k rpm)
15% axial (0.01875")
0.00074ipt (51.1ipm)

Finishing:
1000SFM (30.5k rpm)
150% axial (0.1875")
10% radial (0.0125")
0.00176ipt (161.0ipm)

I've helix bored with tools longer than 12xd before, you just have to go really light on the stepdown. In your case probably around .010" then do the suggested speed and feed.

As an aside I've never found Harveytool stuff to cut particularly quite. Especially they're long reach stuff, for longer reach applications in aluminum I like the Destinytool Viper ERS line they have out now.
I have the same opinion of the long reach Harvey Stuff - I usually don't go with them for this sort of thing. I made the mistake of telling my tooling supplier just the specs I needed - I've had better luck with Helical long reach tools. I kind of put myself into this situation...

I will look into the Viper ERS, though. I found a helical tool in my tool box that fits the bill. I forgot I had it. I will report back with the results.
 

MCritchley

Hot Rolled
Joined
Mar 22, 2007
Location
Milwaukee
I run quite a few helical reachers, their numbers are complete BS and chatter with their settings. Their values start to be close to ok above a half inch cutter. Your run out value is really good, hard to get a lower value.

This be painful but slow down to 30% of what they recommend sfm wise. Keep your chip load up.

I’m only running a few parts typically so the extra minute doesn’t matter.

Sumitomo makes some really nice flat bottom drills that will hold a few thou. from nominal. Won’t help today but their out there.
 

gkoenig

Titanium
Joined
Mar 31, 2013
Location
Portland, OR
This be painful but slow down to 30% of what they recommend sfm wise. Keep your chip load up.

This, 100%.

Every time I've tried to run book rates or even HSM Advisor speeds/feeds on long reach stuff, it never works. Only solution is to throttle the SFM way down and take forever. I think all the S&F tables are just copied from standard length tools without a whole lot in the way of thought.

Edited to Add: I just checked HSM Advisor; the algorithm seems to index on tool deflection, but doesn't take into account whatever the deal is with long reach tools and harmonics/chatter. So it isn't exactly ignoring the length, just the dynamics of the cut that make standard feeds/speeds successful. Would be interesting to track this down and figure out some sort of rule set.
 
Last edited:

guythatbrews

Hot Rolled
Joined
Dec 14, 2017
Location
MO, USA
Several folks make flat drills. I use Kennametal. The are double margin and have a small corner chamfer, maybe .015" on a 5mm drill. They work absolutely great. I think some other makers don't have a chamfer.

Don't know your diameter tolerance but with care and in a pinch you can hand sharpen a HSS drill to cut flat. You'll have to thin the point. Drill as deep as you can with normal drill. Even leave a divot in the middle if you can. Then finish flat with the flat drill. Use normal feed until within .005 or so of the bottom then slow to .001/rev.

Try the flat drill on a scrap piece first. You don't mention quantity but if only a few use oil.
 

Orange Vise

Titanium
Joined
Feb 10, 2012
Location
California
The feature I'm creating is a 5mm Diameter, flat bottom hole. It's 27mm deep. I am drilling out the center with a 2.26mm Drill before the roughing.
Why not use a much larger drill? Like a 3/16". Should help immensely.

Also reduced RPM to 15280 (500 sfm), with the same feed per tooth and no luck.
Keep going down if necessary.

I'm using Harvey 879308-C8 (DIA 0.125, .187LOC, 1.500RCH, 3FL, - V-Helix with TiB2 coating). It's 12X Reach.
That tool doesn't seem to be relieved. It'll be rubbing the whole way down.
 

boosted

Stainless
Joined
Jan 4, 2014
Location
Portland, OR
12XD at that size shouldn't be too bad.

I would helix really small; like start at .002in DOC on a helical interpolation cycle. Then simply increase DOC until it reaches an unacceptable amount of chatter. You should be able to run around .010in at that size, as long as it's been drilled out first.

Can't agree more that Harvey tools seriously underwhelm. The catalog is great, but if you can find the same reach with another manufacturer it will probably cut better. Often you can change like-for-like, and with the same exact cutting parameters; the chatter just disappears.
 

Rcgiovannani

Plastic
Joined
Apr 6, 2015
I run quite a few helical reachers, their numbers are complete BS and chatter with their settings. Their values start to be close to ok above a half inch cutter. Your run out value is really good, hard to get a lower value.

This be painful but slow down to 30% of what they recommend sfm wise. Keep your chip load up.

I’m only running a few parts typically so the extra minute doesn’t matter.

Sumitomo makes some really nice flat bottom drills that will hold a few thou. from nominal. Won’t help today but their out there.
I will try running 30% SFM tomorrow morning. I told the customer I will be late...hate doing that, but I don't ship junk.

Harvey makes flat bottom drills - I will look into Kennemetal and Sumitomo FBD's as well. Harvey is local so I would have it Tuesday though.

Why not use a much larger drill? Like a 3/16". Should help immensely.


Keep going down if necessary.


That tool doesn't seem to be relieved. It'll be rubbing the whole way down.

I tried a 4.5mm first. I was thinking the load on the tool was too small, causing chatter. I've had luck in the past with increasing radial depth of cut with long reach tools. Didn't work in this 1000 series aluminum though.

I think it is relieved. The neck is .120" diameter.
 

Rcgiovannani

Plastic
Joined
Apr 6, 2015
12XD at that size shouldn't be too bad.

I would helix really small; like start at .002in DOC on a helical interpolation cycle. Then simply increase DOC until it reaches an unacceptable amount of chatter. You should be able to run around .010in at that size, as long as it's been drilled out first.

Can't agree more that Harvey tools seriously underwhelm. The catalog is great, but if you can find the same reach with another manufacturer it will probably cut better. Often you can change like-for-like, and with the same exact cutting parameters; the chatter just disappears.

Yeah, and I did try the Helical tool with same specs. I couldn't get it to runout as good as the Harvey tool but it was better. Still not good enough but better. I was running it at 27k though, so like everyone is saying - I will reduce SFM like crazy. I tried helical at like .0025" pitch - maybe it will be better at 30% SFM.
 

boosted

Stainless
Joined
Jan 4, 2014
Location
Portland, OR
Yeah, and I did try the Helical tool with same specs. I couldn't get it to runout as good as the Harvey tool but it was better. Still not good enough but better. I was running it at 27k though, so like everyone is saying - I will reduce SFM like crazy. I tried helical at like .0025" pitch - maybe it will be better at 30% SFM.

1 - Helical is now the same company as Harvey, so for me any long reach tool from them would extremely suspect.

2 - Helical has a bunch of different aluminum specific grinds, and some of them are not so great. For instance, the 35 degrees are fine for roughing, but don't have a lot of stability in any reaching condition.

3 - I would recommend this tool from MITGI if you want to stick with .125in tools. Should be a direct swap.

In my shop we interpolate close tolerance holes in 6061/7075 with 12XD tools several times a month. We stock a bunch of them in the tool crib, and have standard feeds/speeds that work consistently. I just pulled the database for a .125in 12xD: 450SFM, .0005in feed, .002in pitch
 

Rcgiovannani

Plastic
Joined
Apr 6, 2015
1 - Helical is now the same company as Harvey, so for me any long reach tool from them would extremely suspect.

2 - Helical has a bunch of different aluminum specific grinds, and some of them are not so great. For instance, the 35 degrees are fine for roughing, but don't have a lot of stability in any reaching condition.

3 - I would recommend this tool from MITGI if you want to stick with .125in tools. Should be a direct swap.

In my shop we interpolate close tolerance holes in 6061/7075 with 12XD tools several times a month. We stock a bunch of them in the tool crib, and have standard feeds/speeds that work consistently. I just pulled the database for a .125in 12xD: 450SFM, .0005in feed, .002in pitch
Hi Boosted,

Thanks for the info. Do you know what radial DOC you are cutting with those parameters? Like do you make a pilot hole or just slot the helical interpolation?
 

boosted

Stainless
Joined
Jan 4, 2014
Location
Portland, OR
Hi Boosted,

Thanks for the info. Do you know what radial DOC you are cutting with those parameters? Like do you make a pilot hole or just slot the helical interpolation?
We typically pre drill with the closest size drill possible. Often only a few thou under. When I can't or don't want to pre drill I usually drop the pitch even more.
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
A hack to make a good hole in just about any material is to helix-bore it with a high feed. I have 3mm to 3/8" solid carbides on hand, and can get 2mm if needed. It's not fast, but it always works, leaves a good wall finish when the stepdown is small, can be comped in to a tight tolerance, and is good for pretty long length-to-diameter ratios. Bottom won't be fully flat, however.

You can even do it after breaking off a cobalt drill in the work!
 

Blaser Swisslube

Aluminum
Joined
Jul 30, 2009
Location
Goshen, NY
As other users have mentioned, check your coolant, especially concentration percentage. For aluminum, we suggest our Vasco 6000 at 8% concentration.
 

Mtndew

Diamond
Joined
Jun 7, 2012
Location
Michigan
This be painful but slow down to 30% of what they recommend sfm wise. Keep your chip load up.
Yep.
Long end mills are a totally different animal. The key is to find it's happy place, speed and feed-wise and the window is small.
But once you do find the happy medium, be sure to write down the speeds, feeds, and d.o.c and material that you used for future reference.
 








 
Top