Edging – peripheral milling... pleeeease help!!!

hoezap · Aug 23, 2015

Hello

Thank you for entering in my post

I am currently machining mild steel plates 1400x700x50mm.

They do not have a normal rectangular shape, and they have been laser-cut by leaving 4mm of material each side
I need to machine all this profile first, and I am using this 50mm Iscar shoulder end-mill (90 degrees) here on this link
ISCAR Cutting Tools - Metal Working Tools - H490 F90AX-17 : 3104418 - H490 F90AX D050-4-22-17

I am machining these plates on a 8 meters bed CNC milling with a cad/cam program, which cannot be modified, made by my team-leader.
He did set the following parameters: cutting speed 1200rev/min, feed 1500mm/min, cutting depth 2mm; so 25 passes and it takes very long to machine all this profile.

I my company to do profiles, we do always set a small cutting depth between 2 to 3mm and we put a high feederate, I do the same too, since I was taught in this way when I had my apprenticeship.

I know that a maximum chip thickness is the most important parameter for achieving a productive and reliable milling process.
Which would be the best parameters to achieve the maximum chip thickness on this job?
Could I set a 15mm cutting depth, or at least more than 5mm?

I know that using a bigger cutter would help to increase the chip thickness, and I do also have 125mm Iscar shoulder mill with exactly the same tips of the 50mm-one (see link above), could I use it to machine this profile?

In my company they never use extended flute cutters for profile milling, even if we have some of them, (I did put an example on this)
link)ISCAR Cutting Tools - Metal Working Tools - H490 SM-09

Which is the most productive way to machine these profiles?

Any suggestion according this matter will be very appreciative

Thank you in advance for your support

DMF_TomB · Aug 23, 2015

parameters

hoezap said:
Hello

Thank you for entering in my post

I am currently machining mild steel plates 1400x700x50mm.

They do not have a normal rectangular shape, and they have been laser-cut by leaving 4mm of material each side
I need to machine all this profile first, and I am using this 50mm Iscar shoulder end-mill (90 degrees) here on this link
ISCAR Cutting Tools - Metal Working Tools - H490 F90AX-17 : 3104418 - H490 F90AX D050-4-22-17

I am machining these plates on a 8 meters bed CNC milling with a cad/cam program, which cannot be modified, made by my team-leader.
He did set the following parameters: cutting speed 1200rev/min, feed 1500mm/min, cutting depth 2mm; so 25 passes and it takes very long to machine all this profile.

I my company to do profiles, we do always set a small cutting depth between 2 to 3mm and we put a high feederate, I do the same too, since I was taught in this way when I had my apprenticeship.

I know that a maximum chip thickness is the most important parameter for achieving a productive and reliable milling process.
Which would be the best parameters to achieve the maximum chip thickness on this job?
Could I set a 15mm cutting depth, or at least more than 5mm?

I know that using a bigger cutter would help to increase the chip thickness, and I do also have 125mm Iscar shoulder mill with exactly the same tips of the 50mm-one (see link above), could I use it to machine this profile?

In my company they never use extended flute cutters for profile milling, even if we have some of them, (I did put an example on this)
link)ISCAR Cutting Tools - Metal Working Tools - H490 SM-09

Which is the most productive way to machine these profiles?

Any suggestion according this matter will be very appreciative

Thank you in advance for your support

.
metric parameters converted to inch
roughly
640 sfpm
2" dia
if 4 flute
chip .0125 ipt
feed 60 ipm
4.5 hp
depth of cut .080"
.
you probably can increase depth of cut til vibration breaks corners off inserts. double depth of cut and see what happens. your feed is high for steel but only you can see if the carbide insert corners are breaking off. your rpm maybe can go faster. again you are at machine and only you can watch and listen to how it is going

MaxPrairie · Aug 23, 2015

Get a solid carbide endmill and rough the whole plate in two passes. Leave 10 and come back with a finish endmill. I was cutting steel plate the other day from plasma cut plate. 3/4" 1800 rpm 10ipm .25" radial to rough. Then 1/2" 2600 rpm 30 to 40 ipm .05" max radial. I would rather take 1 cut at 6 ipm than 10 cuts at 60 ipm.

HuFlungDung · Aug 23, 2015

I'd recommend a serrated edge endmill, or serrated inserts in an insert type mill. I would most likely take a conventional milling first pass around the part to avoid damaging the inserts in the hard skin of the part. The serrated inserts cut down on vibration considerably, and allow you to feel that you can safely push the feed rate higher.

I wouldn't go to a larger diameter tool than necessary unless it gives you substantially more cutting edges, because you have to cut the rpm. With a given chip thickness in mind, you can often go at least as fast with a smaller tool because you take more chips per second.

hoezap · Aug 23, 2015

Thank you very much indeed to everyone Great answers

DMF_TomB · Aug 23, 2015

slow hogging

MaxPrairie said:
Get a solid carbide endmill and rough the whole plate in two passes. Leave 10 and come back with a finish endmill. I was cutting steel plate the other day from plasma cut plate. 3/4" 1800 rpm 10ipm .25" radial to rough. Then 1/2" 2600 rpm 30 to 40 ipm .05" max radial. I would rather take 1 cut at 6 ipm than 10 cuts at 60 ipm.

.
50 mm dia carbide insert mill should be able to take 6 to 25 mm depth of cut and i would use carbide insert recommend feed rate and rpm or surface meter per minute rate.
.
if that says 500 to 1000 mm per minute feed per minute i find slowing less than 1/2 recommended feed rate i get shorter tool life. i usually back off on depth and width of cut until i am going at least 50 to 100% recommended feed rate and i find i get better tool life.
.
obviously all he got to do is increase things til insert corners break off suddenly from getting near maximum cutter and part vibration can handle. most programmers start at conservative settings rather than tooling not lasting even one part. it is operator who at the machine finds the maximum rate. bigger tooling and bigger parts often part vibration is the real limit. when you can hear chatter 200 feet away and cannot hold a conversation because of the noise 200 feet away you know real vibration and chatter

gregormarwick · Aug 23, 2015

Inserted shoulder mills like the one you're using are designed to cut the full depth of the insert, with feedrate and stepover determined, or limited by, desired chipload, stability, and machine power.

I don't know where this common notion of running them with a shallow DOC came from - as prevalent as it is, it's absolute bullshit.

The cutter you're using is ideal, the DOC is waaaaay to shallow and your feedrate way too high. You've got 16mm max DOC on those inserts, use it! Start about .15mm per tooth feedrate and see how it looks.

DMF_TomB · Aug 23, 2015

gregormarwick said:
Inserted shoulder mills like the one you're using are designed to cut the full depth of the insert, with feedrate and stepover determined, or limited by, desired chipload, stability, and machine power.

I don't know where this common notion of running them with a shallow DOC came from - as prevalent as it is, it's absolute bullshit.

The cutter you're using is ideal, the DOC is waaaaay to shallow and your feedrate way too high. You've got 16mm max DOC on those inserts, use it! Start about .15mm per tooth feedrate and see how it looks.

.
multiple row helix carbide insert mill can take more depth of cut than height of one insert as the inserts over lap. only a facemill is limited to one insert height
.
my experience with 80mm diameter helix mill is at depth of cut of about 28mm at 3mm width of cut and about 500mm per minute feed the finish left is very rough from part vibration.
.
as many machinist only change inserts on end but the other inserts farther up the cutter need changing too especially if depth of cut is more than 1 insert height

Search

Largest Manufacturing Technology Community on the Web

Search

Edging – peripheral milling... pleeeease help!!!

hoezap

Plastic

DMF_TomB

Diamond

MaxPrairie

Hot Rolled

HuFlungDung

Diamond

hoezap

Plastic

DMF_TomB

Diamond

gregormarwick

Diamond

DMF_TomB

Diamond

Similar threads