Help with machining A-2 tool steel

[bookums69]

Hi
Can anyone recommend feeds and speeds for cutting A2 on a Fadal cat40 VMC. I am using cobalt corn cob roughers, HSS End mills and tiln carbide end mills for a post heat treat precision skim cuts. Any advice would be greatly appreciated.

Thanks
Dan

Similar Threads:

• Machining (turning) M4 tool steel
• Need Help!- Machining M2 steel
• Machining Ground Flat Stock - Tool Steel
• HELP MACHINING TOOL BAR STEEL
• Machining A2 steel

[jfrank3]

High speed - 50 sfm
Carbide - 200 sfm

Asd far as feed rates .001-.002 per tooth depending on cutter size and how good of a finish you need. The roughers should take about double that.

Jim

[bookums69]

However, you were the first to reply and I already cut it. I found a little program called ME consultant, It was very help full and it agrees with you I was wondering if you had any experience with post heat treat machining of A2. It will be 40-45 RC. I have alum\tit\nitrate coated carbide cutters. I have heard that I should run them dry with air. But I am unsure of SFM and chip load. Any suggestions?

Have yourself Great M-Day weekend

Dan

[AMCjeepCJ]

Hi,

I cut A2 and D2 by the ton up to and over 62 rockwell. If you need to remove a lot of stock in a hurry, you can't go wrong with round insert ceramics. I have a 40 taper VMC similar to yours and it cuts great minus the insanely hot chips that are prone to catching things on fire. The finish with ceramics using negative rake is almost to the point of a mirror. You can definitely see yourself very clearly in the reflection when things are running smoothly. Another nice thing about negative rake cutters is that the tool pressure is EXTREMELY low since you are basically not cutting material but rather wiping away melted metal much like a windshield wiper on a car~

Hope this helps although I realize you are probably doing detail work instead of general machining. My experience with other operations besides facing I normally run heavy feed, slow RPM and flood using HSS roughers. Right ATM I'm running 500rpm .500" DOC full width on a .750" 4 flute rougher at I think off the top of my head was 1.6 IPM. I'm pretty sure that is accurate and I have not broken a cutter in approximately 30 parts with 25 left to go.

Each piece gets around 36 grooves cut in the perimeter 1.000" deep and I've had no problems with cutter breakage since I have slowed everything down and increased the feed with the HSS cutters. I'm sure there are better methods to do it but this works and I had a pile of those cutters lying around to use verses buying new tooling.

BTW, on my 2 inch cutter I run 1900 rpm and something like 30-50 IPM or more at roughly .025-.05 DOC. I've experimented with (accidentally) over .125" DOC and it worked just as good but I'm not really brave enough or in a big enough hurry to do that very often, although after doing it by accident, I tried it on purpose and it worked but I was nervous and it increased the tool pressure to the point my fixture started to move but the cutters did not break. Besides, I don't think a 40 taper machine is probably the right piece of equipment for that kind of thing.

I bought indexable carbide counterbores and at the recommended speeds I have not actually EVER changed the inserts and there is no noticeable wear after counter boring hundreds of inches of holes in both A2 and D2. The only reason I have not changed the inserts is because the screws fused themselves into the cutter body and since the cutter has paid for itself several times over, now I'm just curious how long it will actually last before it explodes~

Please post your feeds, speeds, DOC, stepover %, etc. so we know what you had success with~

Later taters,

C

[AMCjeepCJ]

Well crap!

I'm kind of tired but if I did the math right, I'm running 98 SFM in HSS and less than .001" per tooth per rev. That seems kinda high on the RPMS for the diameter and kind of low on the infeed but I'm telling ya, as backwards as it sounds it has dramatically increased the life of my cutters.......oh, I just had a brainfart, I'm using cobalt not HSS. Oh well, I'm too lazy to erase this and start over, so sorry if I confused anyone in my earlier post.

I do think I could double my feed per rev with no trouble but these parts HAVE to get done and they are cutting fast enough I don't want to mess with the setup at this point.

Yeah, I was thinking HSS because I knew I wasn't running carbide on this job but I forgot that was a pile of cobalt roughers I grabbed and NOT HSS roughers.

Sorry for the confusion...

Carl

[AMCjeepCJ]

If I forget to post something again, I'm just going to leave it out!

On ceramics I know you need to run chilled air to keep the cutter body cool and to keep the inserts from breaking from thermal shock. I would bet you are correct with running air on coated carbide. I think I'd start there myself and change tactics if things aren't cutting smooth.

On the flip side, I run a lot of 400 series SS in the same hardness area you are talking but with SS I typically bury the cutter, flood it and take a pretty heavy cut to avoid work hardening the SS and have had no problems provided I predrill my plunge points prior to machining.

Please let us know what you ended up doing. For what it is worth, I bought a welding helmet chiller that runs off of compressed air and mounted it in my mill. It works fantastic! I have no idea how it works, I don't believe it has any moving parts, it just has a jiffy connect inlet and two outlets. One that exhausts hot air and the other uses regular pop together coolant lines to blow cold air onto your cutter body. I don't blow it on the chips, I typically aim it straight onto the cutter body or holder itself as recommended by the Ingersol engineer I brought to the shop to test alternate cutters for cutting A2 and D2. Took us most of a day but when we were through we were taking off 50+ cubic inches of D2 per part at 63 Rc in around 32 minutes. My tooling costs were in the neighborhood of $4 to $6 per part if I remember correctly. I'm no expert but I was perfectly happy with that so I spent $1,500 to tool up.

Just remember to listen to your machine, it will tell you pretty quickly what it likes and doesn't like. I was taught how to machine everything on manual equipment and it was easy to adjust infeed, rpm's and DOC on the fly but with my big mill the best I've come up with is to put the bony part of my forehead against anything solid on the machine with my eyes closed and listen to the faint noises and feel the cutter by the way the machine vibrates against my skull. Just keep your hand on the overrides and adjust them up and down, there are always going to be sweetspots that cut great and sometimes they aren't where you expect them. I've found that to be much better at helping me dial in cycle times than any calculations after I get everything setup in the right ballpark.

I doubt I helped much but without knowing the diameter of your cutters, the amount of overhang you're dealing with, the maximum depth you're cutting, if you are going to be side milling with a 1/4" of flute or 2" flute, etc. It gets really hard to give any better advice than just random experiences. Fixturing is going to play a big part too. If you're finishing a pocket in a cavity block is going to machine way differently than if you are milling the outside of fairly hallow part.

I realize you already know this but I'm kind of just guessing as to what type of a piece you are producing. From the little bit you mentioned it sounds like it's a tight tolerance, 'one off' piece that needs to be done right verses right now.

I'm glad it seems to have cut good, can't beat it when everything comes out as expected!

[bookums69]

you guys are GREAT

Dan