Milling with Insert Cutters_ Plunge or Ramp?

[gcode]

Material: hard steel, stainless steel, Ti etc

 

You are milling a feature that is not a pocket.

 

It is possible to rapid to Z depth and then feed into the cut.

 

Question: will you get better insert life rapiding to Z then entering the stock or helix ramping into the material?

 

I've read that its better to helix ramp into the cut instead of just wacking into the side of the part at the desired Z depth.

 

It seems to me, that this would increase cycle time. 2 or 3 helix circles at feedrate take much longer than a Z rapid to depth.

It also makes sense that the helix ramp's

gradual entry into the work would transmit less

shock to the insert.

 

I'd be real interested in some real world experience on this subject.

[edmBosto]

gcode,

When they machine hardened steel at our place for mold components,that have shutoff forms with angles we are forced to use ball endmills.

We always rapid to Z depth and then feed into the cut for this situation.

Sorry I can't compare with the ramping.

[john316]

.

 

I haven't used the open pocket scenario for clearing out material, but in cases where I was doing pocket milling in hard material, where some people prefer to drill an entry hole for the cutter, I prefer to ramp into the pocket with the tool. For me, that is one less tool for the machinist to maintain, and for what you are asking, I've never had any problems with the tool wear as long as my ramp angle and feedrate were sufficient for the tool. I usually use 1.5 degrees on my ramp angles and about 25 percent for the ramp feed.

 

.

[New Job]

In ref. to entering material, I prefer to ramp when I can. After some extensive testing with Ingersoll a few years back we found that the greatest chance for an insert to breakdown prematurely is when the d.o.c. remains constant. An area of stress develops at the point where the material divulges from the insert, and if this point remains constant on the insert, can cause premature wear. You have to find the break even point on tool life versus cycle time. Ask yourself questions like: "Is saving 6 minutes (or whatever time) worth the increased tooling cost?"

 

HTH

[Guest]

+1 dcapps

 

So you add a minute or 2 but you save by not having to stop as often to change worn out inserts.

 

Where I don't do a lot of high production work, I'd say 70% of our lot sizes are 5 or less, I never worry about an extra minute or 2, we will make or break the job on our setup times.

 

Ramping is almost always the way I approach a material entry move.

[Tim Johnson]

I would think if the feature is being profiled and the cut less than 1/2 dia or if the feature is being faced and the cut less tha 2/3 dia ramping is a waste of time. If you're going to use close to full dia then ramping would probably be the better way to go.

 

I would recommend never ramping into 300 series sst unless you use coolant thru tooling or are taking a very shallow doc.

[crazy^millman]

Tom when I am doing closed pockets I like to ramp into the part in that type of materail. If it is an open pocket and I have room I will start as a full depth of cut and have never seen bad results either way. I know people who like to drill a starter hole then following it with the tool. I find this waste more time and collets chips in the whole which beat on the insert causing more problems. Have you guys looked at highfeed cutters for doing this work. When using them ramping is a good apporach for going into a hole and doing it at 100% is what seems to work best. It is good becuase you are never more than .1 deep but when feeding at 240 to 300 imp it makes up taken .4 to .6 depth of cuts at 40 to 60 ipm.

 

Talk to you later.

[Guest CNC Apps Guy 1]

I personally prefer the ramping method.

[Hardmill]

The method Ron described is best on open pockets.

If I have a closed pocket I prefer helical moves if geom. permits it,

this way all the cutting force is transmitted into the spindle.

Which is the idea behind high-feed cutters.

JM2C

 

 

PEACE

[Jack Neelands™]

Ramping for me ...I cut outside profiles on a ramp as well ...In the pocket routine make sure you set your ramp to feed rate and not plunge rate as you want to work the cutter and not burn it out by going too slow ...another trick is to set the ZIG ...or the Zag angle to zero so that you have it ramping down in one direction and not back and forth if so desired