• This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn more.
  • Guest,  We want to wish You and Your Family a Healthy, Happy Thanksgiving! Click the "X" at the top right corner to remove this notice)
  • PLEASE: Read the FORUM RULES BEFORE registering!

4

Milling Problem

3
Like what you see?
Click here to donate to this forum and upgrade your account!
10

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#1
I wanted to make a hex ER40 collet block and mounted a piece of mystery steel in the RT chuck, with TS support but I couldn't take very many cuts before the end mill was dull. I have 2 - 3/4" HSS end mills and dulled both of them in only a few short passes on this stuff. I resharpened both and tried again with the same results. I can't get 3 - 0.025" DOC passes over this short piece before the end mill is dull again. Here are a couple of pics.

First one is of the first 0.025" with a freshly sharpened end mill.
1510456235928.png

this one is of the 3rd 0.025" pass (ie a total DOC of 0.075") and I couldn't finish it.
1510456428814.png

I turned this stuff down from some 2 1/2" rusty round bar and it didn't seem to be unusually hard. Yet I can't mill the stuff. Any ideas?
 

4gsr

HM Chief Foreman
Staff member
H-M Supporter-Premium Member
Joined
Aug 8, 2011
Messages
4,404
Likes
2,665
#2
What RPM are you using? Are you using any coolant or cutting oil?

On your end mill, your primary grind looks a little wide, should only be about a max of .030"-.040". The nasty burr it's leaving is telling me that your primary and secondary angles may not be great enough, that could be causing the endmill to dull quickly. Not knowing what kind of mill you are using, for me, I would take the entire cut, leaving about .010-.015" for a finish cut, instead of stepping it as you have done. Your RPM's should be around 200 give or take a little and fee as much as the machine will handle along with some kind cutting oil or coolant. Ken
 

brino

Active User
H-M Supporter - Sustaining Member
Joined
Jan 2, 2014
Messages
2,844
Likes
2,618
#3
You didn't mention your RPM. That (and cutter diameter) will give your surface feet per minute. That could be critical.

-brino
 

markba633csi

Active Member
Active Member
Joined
Apr 30, 2015
Messages
1,318
Likes
526
#4
Gotta use oil for sure and a slow speed. If you had a cobalt M42 end mill it would help a lot- a roughing mill for example
Mark S.
 

Silverbullet

Active Member
Active Member
Joined
May 4, 2015
Messages
2,357
Likes
1,062
#5
How did the chips on the lathe cuts act and color , what tool hss or carbide.? If you cut it on lathe it'll cut on mill. Try a fly cutter with carbide lathe tool .
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#6
Thanks so much for the reply's. I'll try to answer all of the questions.

The end mill is 3/4" diameter HSS with 4 flutes, it was running at 475 rpm, which is close to what I calculated using the typical formula (did I get it wrong?). I started the feed at about 5" per minute but quickly slowed way down because the chips started coming off blue. The thing I find weird is that these are the same end mills I used to surface a 4" x 6" block of steel yesterday and that went well using the same speed and feed rates, using one end mill for both sides. Different piece of material though. The end mills were sharpened using the same jig, with the same angles, for both projects but for some reason this one is not going well.

The mill is a King PDM 30 ( same as an RF30 / 31, I think).

I'm not using any lube or coolant. I don't use any on the lathe either and it seemed to work ok there (not an excuse; just pointing out the way I do it .... right or wrong). Although I did have to resharpen the HSS cutter many times during the cutting operation. Is there something I can brush on? I'm not set up to use flood coolant on either machine.

Ken, I'll check the width and angles tomorrow.
 

brino

Active User
H-M Supporter - Sustaining Member
Joined
Jan 2, 2014
Messages
2,844
Likes
2,618
#7
it was running at 475 rpm, which is close to what I calculated using the typical formula (did I get it wrong?)
Nope not wrong, I get about 400 rpm for those parameters too.

Is there something I can brush on?
For cutting steel, I use a can of this from the local hardware store in the area with black pipe and fittings.
They sell it for pipe threading.
http://homehardware.ca/en/rec/index...7n/No-216/Ntk-All_EN/R-I1142043?Ntt=oil&Num=0

-brino
 

terrywerm

HM Shop Foreman
Staff member
H-M Supporter-Premium Member
Joined
Oct 21, 2012
Messages
3,529
Likes
889
#8
My methods are not always perfect, but I would definitely be using some sort of coolant or cutting fluid. You might want to build or purchase a no fog coolant mister and use something like Koolmist or Rustlick Syncool. Optionally, you can use a cutting oil like Mobilmet 766, available from Amazon, McMaster-Carr, or MSC. Another cutting lube that works very well, especially on hard materials, is Anchorlube. It is a green paste-like substance that you brush on, a bit expensive, but great stuff just the same. If worst comes to worst, you can always use plain old dark cutting oil, often available at your local hardware store or plumbing supply. It tends to smoke quite a bit though and creates a rather nasty smell in the air, definitely not recommended if your shop is in your basement.
 

Billh50

Active User
H-M Supporter-Premium Member
Joined
Jan 26, 2015
Messages
1,765
Likes
1,170
#9
From reading this thread. I would think the endmills do not have the right reliefs. That or the material is work hardening from lack of coolant.
 

Reeltor

Active User
Active Member
Joined
Nov 18, 2014
Messages
737
Likes
308
#10
How big a bite are you taking (depth of cut)? If your end mill is dulling quickly can you be rubbing on the work and not really cutting?
 

Wreck™Wreck

Active User
H-M Supporter-Premium Member
Joined
Sep 29, 2014
Messages
1,918
Likes
1,463
#11
Climb mill it if possible, from the look of the burr in the picture chip thinning may be at work which never ends well.
Increase the feed rate and step over.
 

Technical Ted

Active Member
Active Member
Joined
Nov 5, 2016
Messages
195
Likes
231
#12
What brand of end mill are you using? I'm asking because I bought some inexpensive end mill from China. You get what you pay for! I have to run these MUCH slower than a good USA brand. If the end mill says HSS with an AL after it you're going to have to slow things way down IMO.

I can take the cutting edge off one of these Chinese mill very quickly if I don't run it about 1/2 the speed, or less, than I run my good ole M42 cutters.

I have a small chop saw that I use to cut the bad ends off my end mills and this is where I can really tell the difference! On the Chinese mills I can cut through them like butter. The nice USA quality brands I get past the flutes and the grinding wheel just sits there and burns until the metal gets red hot and then it will cut the rest of the way though...

YMMV,
Ted
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#13
For cutting steel, I use a can of this from the local hardware store in the area with black pipe and fittings.
They sell it for pipe threading.
http://homehardware.ca/en/rec/index...7n/No-216/Ntk-All_EN/R-I1142043?Ntt=oil&Num=0

-brino
Thanks Brino. I'm going into the city on Tuesday and will pick some up. Do you just brush it on?

DOC ..... I initially tried taking 0.050" passes but found it was too much, then went to 0.025" but the problem persists. The end mills are chinese and are labeled HSS (no AL) on the end mill.

This is the jig I use to sharpen the ends (courtesy of Harold Hall) and I checked the settings again this am. Primary cutting angle is 5* secondary angle is 25* and the rake is 2*.

1510504785716.png
1510504833539.png

Here is a pic of the 2 end mills that are now dull.

1510504921417.png

Wreck - what is "chip thinning" and how is it avoided?

Billh50 - is there a simple way to determine is that is the case? Like a file test? I kind of think that is what is going on but I don't have the experience to know.
 

Bob La Londe

Active Member
Active Member
Joined
Apr 19, 2014
Messages
237
Likes
127
#14
Can you mount the work piece differently so you can use the entire side of the end mill? This would remove more material with less of it passing over any particular part of the mill. Often tips get dulled very quickly leaving the majority of the cutting tool still good.

I do a lot of 3D detail milling so I have little choice but to use the end of the mill, but yesterday I did a project where I used the side of an end mill that the tips have been completely broken off.
 

woodchucker

Active Member
Active Member
Joined
Nov 25, 2015
Messages
1,022
Likes
645
#15
not enough back rake looking at your setup. leave the edge about 1/32 flat but mildly raked the rest rake up away.
Also while the metal is probably not the problem, consider annealing that piece if you can. It is probably a hard piece of steel.
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#16
Bob; Only problem with that is, if I damage the sides I have no way to sharped them (yet) and the end mill will be useless then. I can easily sharpen the ends though.

Jeff; please explain "back rake". Is that the primary cutting angle or the radial angle from the edge to the center?
I don't think the metal is hard because I can easily file it.
 

Technical Ted

Active Member
Active Member
Joined
Nov 5, 2016
Messages
195
Likes
231
#17
Since they are in fact Chinese end mills, I would suggest slowing things down. I run 1/2" ones at 248 RPM and I use a mister while doing so. Much faster and I've found they dull up quickly on steel. YMMV. You could also try reducing the width of the primary grind a little more to see if that helps. I'd suggest shooting for around .040" max.

Good luck,
Ted
 

Bob La Londe

Active Member
Active Member
Joined
Apr 19, 2014
Messages
237
Likes
127
#18
Bob; Only problem with that is, if I damage the sides I have no way to sharped them (yet) and the end mill will be useless then. I can easily sharpen the ends though.

Jeff; please explain "back rake". Is that the primary cutting angle or the radial angle from the edge to the center?
I don't think the metal is hard because I can easily file it.

All cutting tools wear. Given your propensity to sharpen rather than replace mills I am guessing you have more time than money. (Not intended as a jab or a dig.) If it takes me half an hour (I have no idea how long it takes) to sharpen a 20-30 dollar end mill I have lost money. A 50 dollar end mill would likely have a coating on it, so resharpening it would do me no good. Alleast not for its intended purpose. That makes it the equivelant of a 20 dollar end mill...

Anyway, you will get a lot more use out of your endmills between sharpening and/or replacing them if you use the sides. If you also want to use the tips so you can resharpen them then use the sides futher up away from the tip.
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#19
I just came back from the shop and tried a few things. I reduced the width of the primary grind and I used some Rapid Tap fluid brushed onto the work. I also slowed the feed to about half of what I was doing before. I took one 0.050" pass over a new section. It was better but the finish was horrible and was very uneven. I could see and feel the undulations on the surface. So I took a 0.005" pass, very slowly, using more Rapid Tap and that cleaned up the surface pretty well but I could tell the bit was getting dull again. Just for the heck of it I tried another 0.025" pass but I could feel some bad vibrations starting and stopped the mill just as something moved.

Ted, the next thing I try will be to turn the rpm down plus use some cutting fluid.

Bob, not sure how long I have left on this side of the grass so I can't say if I have more time than money or not, lol. But being retired and the cheap SOB I am I prefer to sharpen the end mills as opposed to chucking them out, especially the way things are going for me with this project. I could never do this for money because I am waaaaaaaay too slow and inexperienced but if I were capable and wanted to earn money by machining I would certainly not be dicking around with cheap tooling and spending hours or days making jigs, collet blocks, lining tools, etc. I understand your point about time being money and when I was working, time was a very valuable commodity. This is a hobby for me and most of the time I really enjoy making something from scrap yard steel. It's a great learning experience but can be very frustrating at times. Glad I can get help from the members here or I would probably just go back to one of my other hobbies.
 

4gsr

HM Chief Foreman
Staff member
H-M Supporter-Premium Member
Joined
Aug 8, 2011
Messages
4,404
Likes
2,665
#20
Slow it down! Get the RPM down to around 175-225 and you need some kind of cutting fluid to help. If that is a piece of 41xx and heat treated, you need to cut the RPM's in half, just my rule of thumb I use.
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#21
Slow it down! Get the RPM down to around 175-225 and you need some kind of cutting fluid to help. If that is a piece of 41xx and heat treated, you need to cut the RPM's in half, just my rule of thumb I use.
Thanks Ken. I'll give the slower speed a shot on the next attempt plus I'll brush on some of the Rapid Tap fluid until I can get some proper cutting oil.

Pretty sure it's not heat treated steel. Not positive though. I can easily file this, even after milling it.
 

Bob La Londe

Active Member
Active Member
Joined
Apr 19, 2014
Messages
237
Likes
127
#22
Rapid Tap isn't bad cutting oil. I have some and I use it for that since I decided I like Tap Magic better for tapping.
 

woodchucker

Active Member
Active Member
Joined
Nov 25, 2015
Messages
1,022
Likes
645
#23
Bob; Only problem with that is, if I damage the sides I have no way to sharped them (yet) and the end mill will be useless then. I can easily sharpen the ends though.

Jeff; please explain "back rake". Is that the primary cutting angle or the radial angle from the edge to the center?
I don't think the metal is hard because I can easily file it.
The back rake an angle away from the edge of the cutting tool.it's clearance. The edge should be relatively flat at the tip, but probably 1 degree from flat, then after 1/32nd it should be more like 5 degrees. This is necessary so you don't overheat the edge by dragging it across the metal. There are probably a few people here with better geometry numbers than my guesses, but you want strength in that edge so a very modest angle, then you want a more aggressive angle since it is not doing anything and you don't want chips or uncut metal if plunging being caught in there and dragging
 

brino

Active User
H-M Supporter - Sustaining Member
Joined
Jan 2, 2014
Messages
2,844
Likes
2,618
#24

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#25
Success!!!! :cheerful:

I sharpened one of the end mills again but this time kept the landing much smaller. I reduced the RPM to 215, reduced my feed rate and used quite a bit of Rapid Tap and voila ....... I'm back in business. I cut one new flat from scratch then went back and finished up 3 others and got most of the way through a 5th flat before I started getting shaking / heavy vibrations. Stopped for the night and will resharpen the end mill tomorrow before finishing off the flats. Then I'll take a pic just to prove it really happened and to show all of you what your input allowed me to do. THANKS for all the help!!!!!

Edit. Brino posted while I was typing. Thanks Brino and that is a great reminder to keep in the shop. Things can go very badly in an instant. I've got a pic of my finger after it touched the grinder a while back. I'll see if I can find it and put in the same thread as yours.
 

Wreck™Wreck

Active User
H-M Supporter-Premium Member
Joined
Sep 29, 2014
Messages
1,918
Likes
1,463
#26
A simple explanation may be found here http://www.harveyperformance.com/in-the-loupe/combat-chip-thinning/

However climb milling is difficult on a manual machine, not impossible but will take some effort and planning.
You will find that climbing results in superior surface finishes and less tool wear. Please note that climbing on a manual machine can end in tears so plan ahead.
 
Last edited:

Technical Ted

Active Member
Active Member
Joined
Nov 5, 2016
Messages
195
Likes
231
#27
I agree with Wreck Wreck that climb milling can be "tricky"... If you have any slop in your lead screws it can be a quick way to lose a cutter. It seems to be even more tricky when running cutters at slower speeds. They seem to grab and climb more and you can say goodbye to the corners of the mill or maybe even half the cutter! :eek:.

I usually only climb mill while taking very light finishing cuts where I want a nice finish. You usually can get away with this.

So, I would suggest anyone new to machining to avoid climb milling, unless maybe you're running a nice, tight CNC with feedback control or a manual machine that has a back-lash elimination set up and have it properly adjusted.

YMMV,
Ted
 

HBilly1022

Active Member
Active Member
Joined
Dec 22, 2015
Messages
395
Likes
597
#28
I have a lot of backlash in my machine but did manage to get most of the milling done using climb milling. I kept the DOC to 0.050" for most of the work. I tried some 0.090" DOC towards the end but I was getting some scary feedback and decided to stop and regroup. Will resharpen end mill and finish the job with small cuts.

Ted, what do you consider a light finishing cut? I'm asking because I don't know what is considered appropriate.

Wreck - thanks for that link. I have been milling with about 75% of the cutter engaged in the cut and will try 50% on the next run. By the way, after I reduced the speed, feed and used lube I didn't get any more of those long strands.
 

ericc

Active User
Active Member
Joined
Dec 24, 2013
Messages
240
Likes
56
#29
Success!!!! :cheerful:

I sharpened one of the end mills again but this time kept the landing much smaller. I reduced the RPM to 215, reduced my feed rate and used quite a bit ...
Hi. What does "landing" mean? Is it the same as "land"? I was only familiar with primary and secondary clearance. So, is landing the small flat before the primary clearance?
 
Last edited by a moderator:

markba633csi

Active Member
Active Member
Joined
Apr 30, 2015
Messages
1,318
Likes
526
#30
I've also found chinese endmills to be disappointing for use on steel. Buying good used lots of USA mills on Ebay works for me and saves $
Mark S.
 
Last edited:
6
5 7