What's new
What's new

Maraging 300 Steel, thin steel part, need some thoughts

laminar-flow

Stainless
Joined
Jan 26, 2003
Location
Pacific Northwest
I have a part to machine that is Maraging steel 300 which is like 17-4PH. My plan is to use a Sandvik VCGX 11 02 02-AL H10 which has a small radii and sharp. We only have to rough the part as it will be finished with several OD grinding ops. Probably leave .015 on each surface. The material is .500"Ø and in the soft state. The plan is to hold in a steel jaw air chuck and a center in the tailstock and machine from the center to the chuck, then flip and repeat. Final diameter in the center is about .220". My concerns are chatter and tool life. Sandvik recommends 200-300 SFM and .004"-.008" feed. Not sure on depth of cut but it can't be too much because of cutting pressure. Just 15 parts so speed not and issue only tool life. Any thoughts?

The image shows the tool path and insert cutting one half just over 4.000" long. The total length of the part is just under 9.000" long.
 

Attachments

  • ROD.jpg
    ROD.jpg
    130.1 KB · Views: 105
I would be concerned the pressure from the tail stock will cause it to flex. I think making one will suck, making 15 will suck 15 times more. Why not just get a Swiss shop to do them?
 
We make a part very similar. Out of 6061. But it has a smaller diameter. We rough it out tailstock to chuck to the smallest diameter we can that it doesn't flex. Then retract tailstock and re-advance it. When advancing the tailstock you have to hold the pressure valve and turn the pressure all the way down so the tailstock stops. Then ease it forward by playing with the pressure to creep it up into the part and is just snug. Otherwise it'll crush it. You might have to have someone align it by hand. If you have a stop on your collet or are using soft jaws with a back face, you can clamp and unclamp the chuck to better align the part with the spindle. Then we turn it from tailstock to chuck taking small passes. Using a canned cycle is easier so you can easily adjust your depth of cut. Just play with it. We also use a vnmg insert I think it's a .004" for finish but it's been over a year since Ive seen someone make it and I've never made it myself. This was what my lead at the time and me came up with.
 
Actually sorry don't clamp unclamp. The part I made today you have to do that. Not this other thin one.
 
I have a part to machine that is Maraging steel 300 which is like 17-4PH.
Not so much ... 17-4 is something of a picnic compared to Vascomax, chip-wise. They don't want to break. If you're going to finish by grinding, why not do an inch, push it out an inch, do an inch, push it out an inch ? For 15 parts that might be the easiest. Engine lathe, I hope ? Sometimes nc is a pain in the butt.
 
Well, looks like I might be mildly successful with this part. Wrecked two inserts before I figured it out, sort of...

180 FPM 1200 max, .005 feed, .005 DOC, .030 peck w/ .010 retract. Had to peck to get rid of chips.

I also decide to leave on more than planned as the grinder said they could take off additional material.

Might still tweak it some more but be advised, miserable material this is.
 
Yes, it is a high yield steel when heat treated and it was a pain to machine. If the parts was not so wimpy and I could take a bigger cut the chip might have broke. Had to use peck turn .020 with a .010 retract.
 








 
Back
Top