4130 material

[seawolf217]

i'm working with some 4130 material and i'm not getting a good finish. I'm using a roughing tool taking .05 depth of cut and leaving about .015" for my finish tool. I'm running at around 1000 rpm for rough and 1400 for finish. feed rate is .008 for rough and .004 for finish. I'm running a little slower than i normally would because the part begins to vibrate at the higher rpms. Its a square piece with two cylindrical ends. I'm turning it after the milling has been done. The diameter is ~.5 and the tolerances is +-.0003.

 

Thanks.

[Hardmill]

I think you running too slow.

Start @ about 250 sfm and

quote:

---

because the part begins to vibrate at the higher rpms.

---

increase your chip

load at least 30 %.

 

 

PEACE

[35K chipper]

how hard is your material? RC? if it's in the annel

condition it might give a poor finish.

 

35k

[Ron Branch @ Verisurf]

Look to your fixturing because that would be your biggest problem here. You should be able to run that at 600 sfm with no problem using the right grade and type of insert if annealed if Heat Treated then you are still a little slow in my book if the part is under 1" of the part is 1000" in dia then you are very fast. You don't give a size so depending on what size you are cutting it would be really hard for someone to know if those speeds are god or not. My Roughing would be .200 depth of cut at .026 to .032 per rev, but I am crazy like that.

[GoetzInd]

.032 per rev /QUOTE]

 

I like your style. Sometimes you just got to grip it and rip it.

 

Mike

[ReDEyZZ]

I would start around 4000 rpm and work your way up. 1000 rpm is way too slow for 1/2" diameter.

 

try using a smaller rad on your finish tool if chatter or vibration is still an issue.

[g-codeguy]

I assume you are turning the .5 diameter ends. Only thing I can add to what has already been said is to try a cermet for the finish turn. It will give a decent finish at some pretty slow sfm. Either that or try a ground PVD coated insert.

[BlackOnyx]

4130/4140 as aircraft grade material is supplied annealed, ready to be heat treated to its required tensile strength. Having said that, it can also be supplied pre heat treated to a given state, for example F4. Commercial 4130 is normally supplied at about 28RC. obviously the cutting speed is going to depend on how tough(hard) your material is. Bottom line is, to get a good finish, the insert must be working - if you can't go faster, then increase the depth of finish cut - make the insert work - carbides are designed to shear, not cut (generalization) - the wider the flat on the edge - the more of a roughing insert it is. The chips should be coming off blue - if the chips are sparking, then either you're going too fast, the cuts too deep, or the tip is stuffed. For commercial 4130 (28RC) I would recommend 200 sfm roughing 300 sfm finishing for older grade carbides 300 sfm rough 500 sfm finish for newer grad inserts/cermets (titanium carbide) as a good start point, of course rigidity and depth of cut will have a bearing as well. Deeper cut = slower, lighter cut = faster, it's balance to make the tip work and last. If your getting a **** finish, then the tip isn't working hard enough. If rigidity etc. does not allow suit speed feed, change to a finishing grade. If a heavy finish cut causes tapers, program in counter tapers to eliminate the taper.