[awilliams684]

Hey guys, been lurking here for a while, anyways I have to machine about 60 12' 1 1/4 sq ss bars. I can only machine 18 inches at a time and the bar is supported on the mill over 22 inches the rest is hung over the machine on roller stands.

Ive been on this project for the last week and a half and finally got down to cutting. Well short progress and were already through a pack of inserts which is equivalent to 10 tools and about three bars done (but have to be rerun to fix the finish). Im pretty sure its my cutter that is causing me grief but wanted to get other opinions before throwing more money away in inserts. Im running a 3/4" 2Fl indexable end mill Im running it at 3005 RPM 107IPM .0625 radial .1875 axial DOC no coolant compressed air at the tool.The chips look good slightly tinted but not blued or burned in anyway. I tried to get some temp readings with the infrared thermometer and I saw a peak of about 200F. Spindle load is 10% on a 30HP spindle. The cut is very loud though like the 2fl isnt the best choice. Im thinking about switching to a 3" face mill that uses the same 90 degree inserts that Im using now 6 of them hoping that the mass and increased flutes will help smooth things out.

Ive attached a picture of the fixture on the machine, it is not complete there are 6 edge clamps that run down the length to clamp the bar. The profile of the bar in the picture is what I have to machine. I put a 3" hole in the wall of the machine to feed the bar thorough and leave the door slightly cracked on the other side. A friend of mine thinks sandbags or something similar on the overhang would help combat the vibration that might develop. Anyone with any advice please chime up, it would be greatly appreciated!

[robyward]

Hi, not 100% sure the tool failure or the grade of carbide you are using but if you are going through a lot of inserts on stainless I think it could be a couple of things.

1 - Because of the setup the work piece could be vibrating. Tougher grade of carbides deal better with vibration but wear faster and harder grades will wear better but are more brittle and may chip. If the inserts are chipping then use a tougher grade carbide.

2- If the inserts look like they are burnt which is common on stainless then I would slow down the spindle speed to reduce the insert surface speed on the material and increase the cut per tooth. This will reduce the stainless steels tendency to work harden and insure the insert are always cutting fresh material.

Some more tool information, failure mode and even tool pictures could also help in your description of the problem.

Good luck as stainless can be a pain!!

[PixMan]

You are feeding that with just under .018" feed per tooth. Depending upon the size and design of the insert, that may be up to 2 times what you should be running. Your cutting speed of 590sfm is OK, as long as it's a good grade of insert for that material. If not a good match, that's a bit high.

I think your bigger enemy of tool life is workpiece rigidity. If your photo shows how you're hanging onto this, I can't see how it's clamping the work. Perhaps you should try to add some additional clamping because from your description, things seem to be moving around.

[awilliams684]

Here are some more pictures of the setup, and some of the inserts. Also here is a link to the spec sheet for the inserts I am using.

http://www.mitsubishicarbide.com/mmc...43g_200308.pdf

I can feel a slight vibration in the unsupported bar while machining, but it didn't seem like anything to be alarmed about. I attributed it more to the fact I was using a 2 flute tool. I haven't had any problems with the workpiece shifting etc. The inserts are fine for a while then the spindle load will creep up 1-2% and you can usually hear a change in tone when a chip develops in the insert, so I stop the program replace and restart. I have the tool entering on a 1" radius 22.5 degree sweep I also think some changes in the entry exits could help prolong the tool life. This is my first big job with stainless and Im loosing my a** on it!

[PixMan]

OK, so you're fairly secure in work holding. You are WAY overfeeding the insert if that data sheet is read correctly. Right there it says "0.2mm" as the mean, and "0.1 - 0.3" as the range. That's a max of .0118fpt to your .0178.

If you can get the 6-insert cutter in there and lower the feed per tooth, you'll like the results much better.

[Geof]

I looked at the link you gave and it may be that I am interpreting the information incorrectly but it seems to me your inserts are behaving as they should. Part way down the page is a diagram showing Flank wear versus Cutting length which stops at a cutting length of 15m. What is your total cutting length, it must be comparable to 15m per insert given the shape you are making and the number of passes you do.

[PixMan]

Not the way I see it. The failure mode for the inserts is really hard to determine when you have catastrophic failure like that. What it should be is simple flank wear. What it is, is fracturing. We can't tell if there was plastic deformation, thermal cracking, built-up edge or any of the other common failure modes when the cutting edge is just blown away.

[awilliams684]

OK, so you're fairly secure in work holding. You are WAY overfeeding the insert if that data sheet is read correctly. Right there it says "0.2mm" as the mean, and "0.1 - 0.3" as the range. That's a max of .0118fpt to your .0178.

If you can get the 6-insert cutter in there and lower the feed per tooth, you'll like the results much better.

Before factoring radial chip thinning the FPT was .0098" about 0.25mm. As mentioned earlier the cut is on the heavy side to try to get under the work hardening from the last tooth. After compensating for the chip thinning the adjusted chip load is .0177".

I was looking at these inserts also hoping they are a better grade. http://www.mitsubishicarbide.com/mmc...5tf_200311.pdf

[awilliams684]

I looked at the link you gave and it may be that I am interpreting the information incorrectly but it seems to me your inserts are behaving as they should. Part way down the page is a diagram showing Flank wear versus Cutting length which stops at a cutting length of 15m. What is your total cutting length, it must be comparable to 15m per insert given the shape you are making and the number of passes you do.

There are a lot of passes, that is the program being run. I run 18" at a time and slide the bar 8 times until half is done then flip it and repeat. So cycle time is a concern at 16 cycles per part and 45 parts still waiting for machining, that's a lot of cycles. I was trying to deliver these parts by the end of the week but that doesn't look like its going to happen, I'll be happy just to finish without loosing all my profits in inserts!

[PixMan]

The VP15TF grade just might work better, but what I'd look to for best performance first would be edge prep. If your current insert is showing any signs of leaving work-hardening behind, get a more upsharp edge on the insert.

I don't usually see that much correction factor for chip thinning. Usually, under the depth of cut and width of cut you have there the correction factor would be about 1.3 to 1.4, while you are almost 2x.

[awilliams684]

The VP15TF grade just might work better, but what I'd look to for best performance first would be edge prep. If your current insert is showing any signs of leaving work-hardening behind, get a more upsharp edge on the insert.

I don't usually see that much correction factor for chip thinning. Usually, under the depth of cut and width of cut you have there the correction factor would be about 1.3 to 1.4, while you are almost 2x.

Using the Iscar Excel spreadsheet my correction factor is .5528 I will calculate it by hand and see if I come closer to your numbers.

Is there an easy way to tell if Im work hardening the piece?

[PixMan]

Using the Iscar Excel spreadsheet my correction factor is .5528 I will calculate it by hand and see if I come closer to your numbers.

Is there an easy way to tell if Im work hardening the piece?

The calculation you use should be one specific to your insert. An Iscar calculator may be using a completely different insert geometry that could take far more load.

The only way I know visually to check for work-hardening is color change. I'f it looks like heat got into the workpiece (instead of the chips, as is supposed to happen) you'd see a tinge of a bronze/straw color in 304. And you'd have fast-dying inserts.

[awilliams684]

The calculation you use should be one specific to your insert. An Iscar calculator may be using a completely different insert geometry that could take far more load.

The only way I know visually to check for work-hardening is color change. I'f it looks like heat got into the workpiece (instead of the chips, as is supposed to happen) you'd see a tinge of a bronze/straw color in 304. And you'd have fast-dying inserts.

I will definitely have to check that correction then, thanks for bringing that to my attention. My chips are slightly bronzed, the workpiece shows no signs of discoloration. I think my game plan is to get 2x 2.5" face mills, one a 45 and one a 90 degree. I will run the 45 for roughing and switch to the 90 degree to finish. 5 flutes on each works out nicely with the insert packs since I wont have an odd number left over. Hopefully that will sort me out.

[fizzissist]

Unless you're going to a square shoulder, there's no reason to go to a 90deg insert...you can get higher feed rates, lower entering and exiting stresses on the tool, and better finishes on a 45, AND get better insert life.

One other thing not mentioned is entry and exit toolpath? How you enter and exit is also critical to insert stress loading/unloading. Assuming you're climb cutting?

Vibration is a HUGE issue, btw. I've had times where I've redone a setup to reduce what seemed like just a little chatter give me back double the insert life. ...and assuming your toolholder is rock solid...Which brings us back to insert brand/grade.

I've done a lot of 304, dual-cert, and mostly used Sandvik with pretty decent results. They're actually very helpful when you call with your specifics.

The CoroMill 245 is good for both roughing and finishing, and with a wiper insert you can get excellent finishes. It's a 45deg lead, and I've had good success with the 2030 grade.

[awilliams684]

Unless you're going to a square shoulder, there's no reason to go to a 90deg insert...you can get higher feed rates, lower entering and exiting stresses on the tool, and better finishes on a 45, AND get better insert life.

One other thing not mentioned is entry and exit toolpath? How you enter and exit is also critical to insert stress loading/unloading. Assuming you're climb cutting?

Vibration is a HUGE issue, btw. I've had times where I've redone a setup to reduce what seemed like just a little chatter give me back double the insert life. ...and assuming your toolholder is rock solid...Which brings us back to insert brand/grade.

I've done a lot of 304, dual-cert, and mostly used Sandvik with pretty decent results. They're actually very helpful when you call with your specifics.

The CoroMill 245 is good for both roughing and finishing, and with a wiper insert you can get excellent finishes. It's a 45deg lead, and I've had good success with the 2030 grade.

I do need a square shoulder thats the reason for 90 degree inserts, but if I can remove as much material as possible with the 45 degree that should help save my tool life.

Any recommendations on entry and exits? Im arcing in and out of the cut right now and slowing the feed rate until the cutter is at full radial DOC. I dont see any easy way of increasing rigidity of the fixture without a lot of work which is out of the question.

Im about to order the GMT 2.5" face mills both 90 and 45 degree. The 45 degree will run Kennametal SEHW43A6 Grade KC725M inserts as per Kennametals advice. The 90 degree will run Mitsubishi APMT1604PDER-M2 Grade VP15TF inserts. The main reason for going with these choices is cost and the fact I already have 2 packs of inserts purchased for this job for the 90 degree face mill.

Im going to order in the next two hours if anyone has a better suggestion please share.

[Boltz]

Okay, I looked at that big long tail of the part sticking out there and my first thought was to try milling a section short enough to fit completely in the fixture.
If the tail is wagging the dog it might cause that type of insert failure.

It's possible a very slight change in RPM could tune out the resonance.

But, hey I'm a router guy, so I'm just takin' a wild guess here.

-Jim Hart

[Shane1234]

is insertable the only option available? a 1/2" coated carbide 4 flute endmill could be the solution if you are willing to make .03" side cuts. i run 5500 rpm with a feed of 30ipm, doc at 1", .03" per pass on the side, like peel milling. then the final pass i slow it down. but i get excellent tool life doing it on 304. TaIn coating accupro endmill. speed and feed may very to application, but thats my sweet spot. can pretty much walk away from the machine to do other stuff while it runs, instead of trying to get my mitsubishi to keep inserts in....

[lyfordln]

I found that if you are having a lot of tooling problems, call the Iscar, Valenite, Sandvik, Kennametal tooling person and almost always the person will pinpoint what the problem is. Also, he will have sample tooling to try. Usually the least expensive way to go.

[fizzissist]

Page D11

http://www2.coromant.sandvik.com/cor...1/tech_d_1.pdf

Page D15

http://www2.coromant.sandvik.com/cor...1/tech_d_2.pdf

...note the right pic on D15 showing the cutter moving perpendicular to the cutting path, cutter edge about .08" just off the part and then a radius ramp into the part to begin the straight toolpath.

Sandvik's guideline is starting the perpendicular path alongside the part with the cutting edge .08" away from the part edge, and the radius of the roll-in defined as the radius of the cutter. Width of the cut should be about 70% of cutter diameter....and you want to keep the cutter engaged as much as possible.

...The other thing is that you shouldn't need to slow the feed rate down for entry if you ramp the tool in this way. The ramping compensates.

Hope this helps a little..

[Boltz]

Hey, Fizzy, do you think we can rule out resonance here?

-Jim Hart