pocketing cast iron

[produca2]

Hey guys I am going to run some cast iron parts and will be doing some 2d pocketing about .5/625 deep on 6 inch diametr blanks. I personally have never machined cast iron before and wondered if any of you have any tips before I get started. I will probably be using a cobalt endmill but I am not to sure about that, should I use carbide? I only have cobalt in my larger size end mills so thats the reaon for my tool material choice. Any advice is much apreciated.

[ReDEyZZ]

You can cut pretty easy through cast iron.

 

I would use carbide so you can use a higher SFM.

Don't be afraid to push your chipload a bit, it's pretty soft.(or a rougher endmill)

 

my .02c ,it's dirty stuff, clean your machines good, after the run.

[strabe]

Do not use coolant. Run it dry. I agree with Jarrett use carbide if you can.

[produca2]

why not use coolant? Rust?

[Guest CNC Apps Guy 1]

Because your coolant tank will turn into mud... and rust too.

[Thee Rickster ™]

Cast iron lubricates itself seemingly.

 

don't push the rpm to much because the carbon in it will cause your cutters to wear quickly even carbide.

 

I've done some huge grey cast iron permanent molds

and 'only' used coolant to blast the chips out of rib areas so the small die sinks wouldn't break

(very messy)

 

rick

[Colin Gilchrist]

Thermal shock. Cutting cast iron will generate a lot of heat, especially in the tool. Using coolant will cause the tool to shatter.

[produca2]

o.k. another question, I am using X2 mill level 1 so I dont get all the cool toolpaths that surfaces or solids let you run, so... the part I am pocketing is 6 inch round 1 inch thick pocketed .5 deep with a 1.5 inch dia. boss in the middle. the only toolpath I could get to work was a high speed peel mill following a single circular entity, and just editing the length of the trochoids. Otherwise I cant seem to find a way to run a pocket toolpath without clearing out the boss and everything. can anyone recomend something other than the high speed peel mill, or is the best possible solutioun to my pocketing problem?

[?Mark]

I see no problems using coolant when cutting cast iron. You can lose some tool life, but the work area (vises/fixtures etc...) will be clean. If you run it dry, you're going to waste a lot of time prepping the cycle.

Also, to avoid coolant tank contamination in applications like that I sometimes use landscape fabric as an extra filter

 

Bottom line is not to worry much about tools in this material, as it is very easy to cut, but admittedly very messy.

[Thee Rickster ™]

Are the walls tapered?

are there fillets in the bottom

 

Sound like a simple pocket with a boundary around the boss diameter, unless i am missing something chain the pocket and the boundary for the boss and it should pocket. use ramp for the lead in

 

HTH

[Guest CNC Apps Guy 1]

Have you tried Morph Spiral on the std. pocket toolpath?

[ReDEyZZ]

quote:

---

I sometimes use landscape fabric as an extra filter

---

good tip

 

Cut a hole in it to fit your set-up, lay it out on the table, wrap up when done.

[produca2]

All good ideas I will try and let you know how it goes. Also...if cast iron is so easy to cut why are the speeds and feeds mastercam is calculating for me coming out so damn slow???

[Colin Gilchrist]

Mastercam does not have good material libraries setup by default. The other problem with the material libraries, is that once you get all the values set up, there are % percentage modifiers for almost every aspect of an individual tool. So your SFM could be 1200 by default, but your tool could be set to only use 25% of that value if it is defined as a HSS tool, or 45% if carbide, or what ever.

 

Try this: After you have created the toolpath, open the toolpath parameters dialog box, and right-click on the tool you are using, then select "Feed Speed calculator".

 

This will show you the actual SFM and IPT and will also show you all the % modifiers that are in use. It will also show you the final calculated RPM and Feed Rate.

 

HTH,

[ReDEyZZ]

quote:

---

Also...if cast iron is so easy to cut why are the speeds and feeds mastercam is calculating for me coming out so damn slow???

---

Easy to cut is a relative term i guess, we deal with mostly 4140, 4340, 316 ss,inconel, ect.

 

Carbide endmill of any kind should handle 200-300 SFM. HSS or colbalt 100-150 tops.

[produca2]

quote:

---

This will show you the actual SFM and IPT and will also show you all the % modifiers that are in use. It will also show you the final calculated RPM and Feed Rate.

---

I always do this so I can get a little better feeds and speeds, but jarret is sayin gthat I should be able to run like 2 or 3 hundred ipm with carbide, I am using a 3/8 carbide endmill and my contour feed rate after the feed and speed calc is only 7.23424 with a spindle speed od 2444. I changed the percentage modifier to 100 % even and thats all I get, I dont understand. I am gonna try to calculate this by hand and see what I get. I have a 7500 rpm spindle so I should get some faster feed rates I believe.

[ReDEyZZ]

quote:

---

2 or 3 hundred ipm

---

"sfm"

not "ipm". Feed rate will depend on the type of endmill. prolly .006-.01 per rev depending on depth of cut.

[produca2]

Never mind, I just changed my SFM in the feeds and speeds calc and it changed everything! I love to learn new things Thanks guys for those valuable little tid bits! I wish I would have known those things before when I was having problems with stainless steel!

[?Mark]

With a good quality carbide endmill (ex. varimill) I'd start (for .375 dia tool and gray cast iron) at S4580 and F30.0 IPM.

If a setup is rigid (tool as well as a part) then those speeds are good for slotting too(up to 100% dia)

hth

[produca2]

I have this thing blasting at 135 ipm at 7500 rpm making .02 deep trochodial cuts! I know I can run it deeper, but I will stay safe for now! thanks for all the help guys! you really helped me out on this one!