I'm recutting chips right? Picture included

[JWB_Machining]

Hey,

So I was doing a contour in a piece of steel with a 1/2" carbide endmill. The piece of steel was about .4" thick and I was take cuts with a 0.1" depth. Obviously chips were building up around my cutter. After I milled the contour I took a finishing pass at the final depth to remove 0.001", obviously my cutter had gone all the way through so it wasn't recutting chips on the finish pass but am I right to assume that on my roughing passes I was recutting chips and this caused the gouges as seen in my picture. What are my possible remedies for this? A Deeper finishing pass or set up a lil jig holding an air gun on my tool as to blow all chips out of the way? It wouldn't be the correct thing to use coolant because i'm using a sold carbide cutter with Ti coating and coolant could cause thermal fracture in my tool correct?

This picture is taken at 50x and it appears that each "gouge" starts with a burn/smear and ends with one.

[Geof]

If you are cutting dry you should have an air blast all the time.

What is the steel, what is your rpm, what is your feed?

A depth of cut of 0.1 is quite small.

You mention cutting all the way through: on material 0.4" thick you could drill through and then do everything at full 0.4" depth with an air blast.

Have you seen the videos I made showing a 1/2" cutter in hot rolled steel in this thread?

Now I'm a believer; you can mill C1018 at 800 FPM

Not nevessarily directly applicable to what you are doing maybe but it shows you what is possible when you grit your teeth.

If you are machining a higher carbon steel you could probably maintain the same rpm but back off the feed.

[JWB_Machining]

The Spec says it's 4340 and I tested it to be about 44 Rockwell C. My Feed was 0.9 and my RPM was 300.

I went with a 0.1" depth of cut because a very wise man (you) once told me that to be safe I should make depths of cut about 20% of my cutter diameter and I've been using that because it's worked wonderfully. Plus I Figure once the contour is done then when I do a finishing pass at the final depth my cutter is still fresh and only the bottom 0.1" of it is worn. I will definitely try cutting at the entire depth in the future I just figured this might cause too much of a load on my tool or something and often if I screw up I've got explaining to do since I often only get one piece of material to have to machine from.

I do drill all the way through the material at the start of my contour and then plunge my cutter into that. You're saying In the future I should try cutting the contour at the entire depth?

Unfortunately we're not allowed to view streaming media here so I'll have to wait till I get home to check out the video. And Just to Check with steel like this I shouldn't have a chip load over .001 correct? Remeber I'm not a production shop here so often extended tool life takes importance over quick cycle time.

Since I've got your attention Geof when do you like to use indexable insert carbide end mills and when do you like to use solid carbide end mills?

[Geof]

Oooh! Hoist by my own petard: I went with a 0.1" depth of cut because a very wise man (you) once told me that to be safe I should make depths of cut about 20% of my cutter diameter

Check dates and I think you will find that advice was given prior to my being converted as the title of my thread says.

Fortunately I included this sentence in my post so I have weasel room to argue I am not really contradicting myself;Not nevessarily directly applicable to what you are doing maybe but it shows you what is possible when you grit your teeth.

Actually I think your figuring about cutter wear is pretty well correct and really the only thing you should have done is put on a strong air blast all the time.

I think your chipload was okay for your material but your rpm may have been a bit low, were the chips coming off discolored or blue?

I sympathise with you regarding tool life and having to explain why things didn't work; I occasionally have to mutter to myself when something doesn't work.

Regarding your endmill question I don't use indexables; mostly because the intial cost of the holder is quite high and the inserts often cost about as much as a solid carbide cutter that can do the job. I have to be honest I do kill cutters every now and then and I would rather kill a $45.00 solid mill than a $185.00 indexable.

[JWB_Machining]

No my Chips were not coming off blue or discolored, I believe I should be pushing my speeds n feeds until I start to get blue chips but my machine/set up did not seem to like to go much faster, I ended up getting mean sounding vibration so I backed off not wanting to wear my cutter too fast or possibly chip the cutter or seize the tool.

I'll definitely get around to rigging up an air blast of some sort for dry cutting because I always dry cut when I'm using carbide in steel.

[John Welden]

Originally Posted by JWB_Machining Hey, So I was doing a contour in a piece of steel with a 1/2" carbide endmill. The piece of steel was about .4" thick and I was take cuts with a 0.1" depth. Obviously chips were building up around my cutter. After I milled the contour I took a finishing pass at the final depth to remove 0.001", obviously my cutter had gone all the way through so it wasn't recutting chips on the finish pass but am I right to assume that on my roughing passes I was recutting chips and this caused the gouges as seen in my picture. What are my possible remedies for this? A Deeper finishing pass or set up a lil jig holding an air gun on my tool as to blow all chips out of the way? It wouldn't be the correct thing to use coolant because i'm using a sold carbide cutter with Ti coating and coolant could cause thermal fracture in my tool correct? This picture is taken at 50x and it appears that each "gouge" starts with a burn/smear and ends with one.

It's proper to rough things out with a roughing endmill and then go back in with a finisher, especially in harder materials.

Normal endmills don't like cutting 180 deg of the cutter. (slot cutting) A rougher is better at breaking the chips up and getting them out when you've got to cut at full width. Do what you've got to do to get get the chips out. Air blast, flood coolant, whatever. Maybe you'll only be able to take a very light depth of cut.

Get the most ridged setup you can. Keep the quill up and use the knee for Z adjustment. Use the shortest endmill you can.

A lot of problems can be from laziness. The quill is down a foot, the endmill is hanging out a mile and your work piece isn't held down well. If you don't start with a good foundation, the rest of the job is a pain in the arse.

When I was an apprentice at a mold shop I would get shot if I had the quill hanging out while milling. We didn't have power knee feed either. Had to get on that knee handle and start crankin.

That whole "thermal fracture" thing is kind of overblown. People worry way too much about it in most cases.

The bottom line is that making end mills do their job isn't magic. If you're having problems, back way up and make sure you're giving the cutter a chance to do its job. Everything will be better when you've got a good set up. Faster,deeper,longer tool life and better parts.

[JWB_Machining]

I'm using a Haas TM-1 so no quill or knee adjustment for me the spindle just lowers into place. But yes I had the end mill hanging out as lil as possible, enough to go the depth I need and not so lil that the set screw of my endmill hold was going into any flutes. As for roughing endmills I just got a bunch in so i'm definitely going to start incorporating them more often. Was playing with them on the manual mill and they defintely remove material faster.

Thanks for the advice and while I've got your attention though, unrelated to this project, it's never correct to clamp a collet down on flutes is it? Also any opinions on drill mills? Got a bunch of them in as well since they were dirt cheap but since they're dirt cheap and claim to be 5 tools in one I feel like that means they just do 5 different jobs all sub par of job dedicated tools.

[John Welden]

Originally Posted by JWB_Machining I'm using a Haas TM-1 so no quill or knee adjustment for me the spindle just lowers into place. But yes I had the end mill hanging out as lil as possible, enough to go the depth I need and not so lil that the set screw of my endmill hold was going into any flutes. As for roughing endmills I just got a bunch in so i'm definitely going to start incorporating them more often. Was playing with them on the manual mill and they defintely remove material faster. Thanks for the advice and while I've got your attention though, unrelated to this project, it's never correct to clamp a collet down on flutes is it? Also any opinions on drill mills? Got a bunch of them in as well since they were dirt cheap but since they're dirt cheap and claim to be 5 tools in one I feel like that means they just do 5 different jobs all sub par of job dedicated tools.

Good to see you've got a TM1, it's a decent little machine. Key word little.

I wasn't trying to lecture you about things that don't apply to your situation. Sorry about that.

You may only be able to take fairly light cuts on that TM1, especially in steel. One way or another, get your work piece roughed out with a rougher or normal end mill. Take small cuts if you have to. It's hard to say exactly what to do without being there. You're going to have to play around.

Get your finish end mill in there and try taking only .05 depth of cut. Work your way down. It's nice to take the finish pass in all one cut but on a light machine you may need multiple passes in Z.

Get a tool holder that doesn't stick out a mile. Get that endmill as close to the spindle as you can. It seems like no big deal to have it stick out a couple extra inches, but on a light machine, you need all the advantages you can get. Think how much leverage you can put on a wrench by adding a couple inches to the handle, vs, choking way down on it. Think how much a little run out amplifies the further you go out. If I was turning a 1/2 bar in the lathe, I'd certainly rather work near the chuck than say, 4 inches away. It will deflect and run out.

Like I was saying, its so hard to give advice when you're not there in the shop. That's why I mostly try to give advice on fundamentals rather than tell you exactly what endmill to use and how fast to go. Try to play around and experiment. Don't take anything I tell you or anyone else on here as the only way to do things. There are a million ways to skin a cat in a machine shop. If you get your parts done in a reasonable amount of time with reasonable cost, that who cares how you did it?

It's not proper to clamp on the flutes of end mills or drills. Is it the end of the world if you do?, no. Another thing to remember is to load your tools well. Clean the damn taper off, clean the spindle, clean the end mill and holder. There seems to be a broad interpretation of what clean is in machine shops. I take a little extra time and clean these things until they are immaculate because it does matter. I wipe the tool taper off before every time I load it and I quickly inspect it for anything I may have missed.

It's back to fundamentals and remembering that everything adds up. A little junk in your spindle, the collet is a little dirty, the end mills is a little dirty and tool holder sticks out a mile. Personally, I'd much rather use an immaculate set up that is as short as possible. The extra time I spend on the front end, pays off huge at the back end. I'm not one of these guys that cleans things immaculate just because I want to be anal about everything. I clean so I can go faster and make better parts, that's it. I don't really give a crap about the machine, I just want it to work as well as it can.

I also use high quality tool holders and end mills. Why buy a nice car and put crap tires on it? Most name brand end mills are pretty damn good these days.

I haven't worked at a shop that needed any mill drill combos for a job. Those are usually more about blasting a bunch of holes in a plate and then interpolating them out. Maybe throw on a chamfer at the same time. For the right job they can be great. I generally avoid combo tools in the machine shop or wood shop. Dedicated tools seem to usually be the way to go.