Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Some questions on milling/turning tool steels


Recommended Posts

Hey there everyone.  Been lurking around here for quite some time and have learned quite a bit.  I've only been programming/machining for a little under 2 years so this place has been a wealth of information and perspective.

 

So, to bore you guys with some details I'm kind of in a unique situation where I've learned this trade from coming from being a 3D animator.  Kind of weird I realize as pretty much every one comes from being a machinist first before migrating to the programming aspects.  I'd like to add that I've learned what I have so far in the trade by cutting a line of products my shop makes which are all made of tool steels and HSS.  So, it's been kind of an unforgiving learning process and I'm a little stuck on what to do about certain situations that I'm hoping some of you can help with and this will probably be a little long.  So sorry and thanks for reading my wall of text.

 

Some pretenses--

 

I cut mainly metals like CPM 9V, M4, 4150HT, H13, and recently Z-Max.  I'm milling on early 2000's Haas VF2 and VF4, and turning on predominantly a similar year ST20 and an SL30.

 

The main issues I'm having here are mostly in the tool wear department.

 

 For turning the biggest issue I'm having is cutting off.  We're a job shop so it's kind of a "you have to use what you've got" sort of situation which doesn't help the issue as we're using sort of random/generic inserts with random geometry and no matter what parameters I use we are changing inserts on our cut off tool after every part or every other part.  I'm only cutting off something with a wall thickness of on the high side of .5".  I feel like this is absurd.  What sort of tool life should I be getting here?  I've tried speeds from 150-300 SFM and .002 to .004.  I've tried pecking, I've tried feeding it straight through.  Nothing really seems to be helping.

 

As for milling making an end mill last in these materials is even worse.  Generally I'm cutting 4 to 6 flutes on a turned piece in a dividing head starting out by opti-roughing generally doing an 8-10% step over and 1.5xDIA DOC and I'll be lucky if an endmill survives 10-15 minutes of cutting.  Sometimes the cut sounds good sometimes it just sounds incredibly rough.  I mean these Haas can barely take a 30% WOC .05 deep in 1018 with a insert cutter without screaming so I'm sort of at a loss here.  I use HSMAdvisor for my feeds and speeds and try to dial in the parameters as closely as possible there but I'm still having massive issues.  

 

Would it be best to run this type of toolpath dry or with air blast?  A while back I had managed to get a TiALN coated EM to make it through 17 parts feeding at like 2x the normal feed rate I do by running it dry through the roughing cycle.  However, I have guys who have been machining for 20-40 years here telling me I will end up work hardening these if I cut them dry.  This seems to be contradictory to my research and that single event/test.  With the complete lack of repeatability I seem to be getting (partially due to the fact that every week I'm having to cut with some random end mill with a random coating and random geometry because that's what was on sale) I'm just lost on what direction to go.

 

Also, we only use/have side lock holders.  I'm wondering if a milling chuck would be a better fit for this type of tool path?  Would that provide some extra rigidity increase tool life?

 

I feel like I'm trying to cut a rock with random pieces of cheese over here and catching flak for using up all the cheese.

 

Anyway, thanks for reading my wall of text and I really appreciate any help you guys can provide.

Link to comment
Share on other sites

Welcome to the forum!

It took me a while to fully agree that getting the correct cutting tool made a huge difference. Getting information from other users on what works well helps. Contacting your suppliers and get them to bring samples in or tech reps from the cutter companies. Call the manufacturer of the inserts for your parting tool and tell them the specifics and see if you have the correct insert and get some conservative speeds and feeds.

Good luck!

Link to comment
Share on other sites

These materials are not new, people machine them all the time. Work on the money spender to buy the proper tools. There are so many good endmills out there now you can't afford to not use them. The competition is, you know how I know? Because we run them. It will save so much money in the long run. Do your best to look at the big picture instead of being short sighted like your co-workers.

 

Milling prefers dry, especially hard so you don't shock the tool. I don't know how big your parts are but if you can swing an inserted high feedmill like this: Iscar FF EWXD0.62-2-1.5W0.62-04 you will be amazed how fast it will run and for how long.

 

As far as the parting tool I like Iscar penta turn.

 

You're doing the right thing, keep learning and there's no telling where you'll be in a couple years.

Link to comment
Share on other sites

Good luck with the CPM 9V, I haven't cut any in about as long as you are old but remember it being tougher at a lower rockwell than most materials were at 58C. Nearly impossible to grind also, that's back when "C" had the patent on CPM9 and 10 and nobody else could make it so it was expensive also.

4150 and H13 will be manageable.

 

The "you have to use what you've got" sentiment I'm assuming from management is counter productive (trust me I weathered it here where I work for years) and is the same thing that lead them into a shop full of HAAS's. You have the potential to be very valuable to your shop if you can step up their game a little and you are on the right track by asking questions here :)

  • Like 1
Link to comment
Share on other sites

Milling prefers dry, especially hard so you don't shock the tool. I don't know how big your parts are but if you can swing an inserted high feedmill like this: Iscar FF EWXD0.62-2-1.5W0.62-04 you will be amazed how fast it will run and for how long.

 

I figured I was correct about running dry.  Going to try to convince them to let me try to right up an airblast.  As for the part size, most of the time I'm cutting .25" to 1.75" slots with full radii at the bottom.  I've been seeing some luck with some millstar ball mills with HSN inserts but the downside is these are about 6x long so feed rate suffers a lot.  Going to try to at the very least get them to invest in some stubbier versions.  So I had been trying to go in with .1875" to .375"  EM to take out the bulk of the material and only use the ball mills to rough out the radii at the bottom to make up some time.

 

 

You have the potential to be very valuable to your shop if you can step up their game a little and you are on the right track by asking questions here :)

 

I believe the unofficial shop motto here is, to quote the great Garth Algar, "We fear change."  :guitar:

 

Thanks for what feedback I've gotten so far, guys.  I really appreciate it. 

 

Link to comment
Share on other sites

I believe the unofficial shop motto here is, to quote the great Garth Algar, "We fear change."  :guitar:

 

If your location didn't say Ohio, I'd swear you worked here. :fun:

 

I recently bought 18 Nikken mill chucks. We were starting out doing "peel" milling, opti-rough, "dynamic" milling, whatever you wanna call it. Got a good feel for how to do it on our better machines, that have better toolholders, then moved it to the roughing department. Broke cutters like crazy using solid end mill type holders. Finally had an operator indicate the cutter in the holder, .006" TIR. Not conducive to great tool life. Also found one poor old Fadal had .008" of backlash in the X axis, again, not a big help.

 

We have had good luck with endmills from Fraisa. Their tool expert calculator is nice and has served us well. Pick a cutter based on material hardness, pick a size, pick low, medium, or high dynamics, usually limited by what your machine is capable of, then pick basic, intermediate or advanced level. That's limited by you and how easily you scare. :laughing:

 

For example, a 1/2" end mill, at 1.5"DOC and .025" stepover, in 24-34Rc steel wants to go 5500RPM and 325IPM when you select high dynamics and advanced. It's fun to watch.

Link to comment
Share on other sites

Helical makes pretty good cutters at a pretty good price, and their milling advisor program will tell you how to use them.  Any steel that isn't stainless should be cut dry with air blast and a TIALN or similar coating, and don't try to back the RPM down a bunch to "be safe".  You need to run it fast enough for the heat to soften the chip; the TIALN coating will protect the carbide from that heat and becomes slipperier at higher temperatures.  You will actually shorten the tool life if you slow it down.

Link to comment
Share on other sites

As far as turning is concerned a good way to get more tool life and rigidity out of your set-up is turn the cut-off tool backwards and run the spindle backwards at an M04 instead of an M03. This forces all of the tool pressure into the bed of the lathe rather than pulling up on it, works like a champ.

Up turning is what they called it in a class I took , work well for real heavy cuts , as you stated applies pressure onto the ways rather than lifting the turret off the ways .

Link to comment
Share on other sites

Be careful of running those milling chucks that have a excessive gage length, esp in a Haas.  I have a couple here that just collect dust...

 

Several different companies make nice precision collet type tool holders for finishing and semi-roughing.  Don't be afraid to use side lock holders for roughing, the good ones have very little run-out.  I really like those super short ER 32 holders where the collet is actually recessed into the taper.

 

Good tooling makes all the difference in the world, yes even in a Haas.  I run almost all steels dry (maybe not 304 or Ti) and it's the only way to fly!

  • Like 2
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...