Milling D2 ring cams

[Smit]

Hi Folks,

I need to make a ring cam from D2 tool steel. The cam is made in four quadrants. The part I'm currently working on is ct from a 3 1/2 x 5 x 11 5/8 block. I'll have to mill this part into its round shape, drill, tap and ream a few holes, then mill the cam slot on a radius. It appears to me a ball mill would be the best way to mill the slot. Has anybody had success milling a slot of this type in D2 before? If so, please share the type of ball mill you used. I would think this application would really eat up carbide ball mills.

 

Also, there is a lot of material that needs to be milled away to cut these parts into a ring. I'm planning on using a vise to hold the parts upright while milling this material, and maybe using a plunge mill to rough it out. Does anybody have a specific tool they prefer to use in D2 that would give better tool life?

 

Thanks in advance for any and all replies!

[Jack Mitchell]

Bandsaw as much material as possible since milling is going to be very tough. I wouldn't plunge rough this personally.

390 Sandvik series cutters (the 1.25" diameter is best with five inserts)layered cuts appr. .03" axial, lots of feed - you will get about a 2 second notice before the inserts go.

Take your time with this project "at the very least try to build some character"

 

Some grades of stainless can be tough, but I would rate D2 as one of the most difficult.

 

 

Regards, Jack

[savagkd]

Heads up on the drilling, D2 work hardens BAD! If you can, drill it with thru coolant, no peck.

 

+1 on the 2 seconds Jack.

 

HTH

 

Keith

[Aaron AKA. Zippy]

Smit,

 

D2 is nasty shiznit but I get stuck cutting alot of it. I have found that if you are useing solid carbide to use one of the variable helix types such as a Z-CARB with TiCN coat. I run 200SFM and keep chipload up around .0025 FPT W/ a 3/4 EM. Run it dry with an air blast, if you remill a chip your cutter is a gonner. I also often use a 3 flute 1" insert cutter at the same speed but keep the chipload up at about .006 FPT. For a face mill I use a 2.5" 5flt 45deg laed cutter still run 200SFM but feed up to .010FPT depending on DOC. If you have the time and not the money I have also had alot of sucses with Cobalt roughers I run 30SFM and .005FPT, if you have the torque at low speed you can burry one 2xDIA deep and 90% on the side. BTW CLIMB cut only!!! even with the face mill.

Works for me... let me know if it works for you.

 

Zippy

[Thad]

Smit,

 

We don't do the kind of work that you mention here. While D2 is some tough stuff, I don't think it's as bad as the others think. We routinely mill D2 with a 2" Teagu Tec or Ingersoll face mill at 1200 RPM and 45 IPM, with a .06 DOC. That's about 630 SFPM and a .012 chip load. We use standard grade inserts with no special coatings.

 

As far as drilling goes, we drill all materials at 2 IPM. We've drilled 5" deep in D2 with flood coolant and a G83 peck drilling cycle with no problems. In fact, I can't recall a time that I work hardened a piece in the last 10 years.

 

My 2 cents. Good luck.

 

Thad

[Aaron AKA. Zippy]

Thad,

 

After seeing what you get away with it makes me wonder if I an doing somthing wrong. I will agree that drilling dosent pose any problems, but the times I tryed higher speeds the inserts would not last. Would you share in greater detail some of your setup such as raidial engagment and what sort of machine.

 

I would also like to discuss grinding it. Maby I should start a new thread on this subject??

 

Zippy

[jbel]

quote:

---

I would also like to discuss grinding it.

---

Ha! Grinding D2 Now that's a good one!!

 

It is the biggest PITA I have ever seen. Any suggestions would be appreciated.

[ChuckM]

I've had very good success with Mitsubishi's APX line cutting D2, D3, A2 and a few other tool steels so far. Inserts are the AO-style with Mitsu's VP15TF coating. For D2, the .75-1.25" cutters generally run at 500-600 sfm (slotting) with .006-.010 ipt, 600-700 sfm (shoulder).

 

For face milling, I use a 2 or 3" Mitsu BRP with .25 radius VP15TF inserts. Being a round insert mill, you have the chip thinning factor to work with but generally we'll use ~.018 ipt for a .060 doc & ~.012 for .120 doc, 450-650 sfm.

 

I'm running these tools on Haas VF-series mills.

 

Other than feed and speed, I think the most important factor to consider is your machining techniques. I follow a few rules with face mills...

 

1) Dry cut, air blast

2) 66% radial doc

3) 50% feed reduction for tool entry & exit

4) climb cut

 

For end mills...

 

1) Dry cut, air blast

2) 50% feed reduction for ramp-in or off part tool entry

3) climb cut

4) when pocketing use a "morph type" toolpath routine

5) use corner override

 

For grinding, rough using a gel bonded ceramic wheel. 20% ceramic Milacron wheels are real good for this. Coarse dress and rough dry in one direction.

 

Finish grind with a Norton 46I or H wheel, doc<.0005, .25-.313 cross-feed.

 

Works well for me.

 

-Chuck

[Thad]

Zippy,

 

I've done very little grinding in my day and even less on D2.

 

My numbers from above are done on a Fadal. I usually go with 60% of tool dia for stepover, use an air blast, and climb cut only. Insert corner radius is either .063 or .125. When I pocket, I use a Constant Overlap Spiral and most parts are just clamped in a vise. These numbers are good when using the shortest arbor, which would make the total tool reach under the flange 2.25 long. When I use the longer arbor that will get me 4.75 reach, I have to turn the feed down to 80-85% on the override. Maybe even go with a .05 DOC.

 

Thad

[Aaron AKA. Zippy]

Well dang!!! seems like everyone but me is haveing a good time at higher speed. I'm going to do some experimenting with some different inserts and whaten and try again.

 

When it comes to grinding there is only two things we grind here, carbide and D2. Due to the ammount of carbide we grind most of our grinders are set up with 240grit reisen bond dimond wheels. We have found that it works best to treat the D2 just like carbide, I plunge grind w/ .0002 pick feed to rough. Then you can pick down up to .001 at a time with .100-.150 crossfeed. We can grind all day without haveing to redress the wheel. Most people look at me like I'm stupid when I tell them this but it realy dose work.

Zippy