[diyengineer]

Have a little part I need to machine down, made of stainless. Any suggested feeds and speeds would be great, along with depth of cut. Area to be machined is 3/4" long x 1/2" wide. Have to machine it down about an inch. Have the superfly cutter and polished insert.


Washington state

[tmarks11]

That will make a nasty interrupted cut with the fly cutter, and you are taking off a lot of material. A flycutter gives you the advantage of covering a large surface area, and giving a good finish quality. With the surface area you are cutting, that first advantage goes away (and buys you short insert life in the process).

Just use a 1/2" end mill.

If you want the finish quality from the flycutter, than get it down to about 0.050" above final dimension with the end mill, than finish it with the flycutter.

Rightr cutter for the right job will make your life better, and make your equipment last longer.

[diyengineer]

Ya, when I was doing it I stopped because the vibration was pretty bad. What feeds and speeds would be suggested for the 1/2" carbide cutter? I usually work with aluminum 2024 so this is the equivalent of milling a rock for me hahaha!


Washington state

[tmarks11]

Assuming 302 stainless:

4 flute cutter, 0.500" DOC, taking off 0.250" on each pass (only using half the cutter, overlapping passes, conventional milling), makes it 12 ipm, 1400 rpm. That gives you 0.9 hp required, 186 sfm, with chipload of 0.002" per tooth.

That is from FSWizard (FSWizard - Free Advanced CNC Speed and Feed Calculator). One of these days, I will buy a copy of GWizard.

Personally, I would probably cut the first pass at 0.250" DOC and see how it went, but than I am a wuss sometimes.

If you are not going to finish it with the fly cutter, than save 0.020" for a last finish pass with the end mill to clean it up.

Another solution is a face mill, assuming you have a small one (3/4" diameter). I dislike the interrupted cutting when hogging off material, but than I am in the business of maximizing tool life, not production.

[diyengineer]

Appears on closer inspection the carbide didn't last long on the fly cutter.


Washington state

[tmarks11]

yeah, interrupted cuts will kill your carbide inserts. The insert just bashes itself to death on the edge of your work piece every time it swings around. A small face mill would probably last longer, since you have at least 1-2 inserts on the work piece through the cut.

The end mill is a better choice because it has teeth engaged continuously during the cut.

Don't have to worry about waking up your family by working early? I need to get a shop separated from the house... it is on my shopping list.

You said you had a "polished insert"? I am guessing that is the uncoated, sharp edged Korloy inserts that Tormach sells for aluminum? Not a great choice, you really want a coated insert, that doesn't have as sharp an edge, and is the appropriate carbide grade for steel and stainless. As expensive as carbide is, it is important to match insert to material when selecting your cutting tools.

That being said, even with the right insert, I suspect you would have chewed it up before you finished cutting.

[diyengineer]

Well goes to show how much I use my personal mill. Seems that somehow the clockwise spindle on button is indeed going counterclockwise which means I ran my insert in the fly cutter in reverse. Idiot... Hahaha!


Washington state

[tmarks11]

Have you noticed that problem in the past? There was another poster here who just got a PCNC1100 (Chrono1124), and his was programmed to run backwards as well.

Really makes it hard to drill neat holes in material... and tool life sucks...

[MichaelHenry]

Have the superfly cutter and polished insert.

The polished insert (P/N 32653) is meant for aluminum. You might be better served with the P/N 32654 insert.

Fly Cutters

Mike

[RussMachine]

Always use the smallest endmill that can get the job done in a relatively fast manner.
Think about it.
If you swing your fist around at arm's length, it will make a hard impact.
If you hold your fist against your chest and swing around, it will barely make any impact at all.
Small diameter = less impact.
Large diameter = hammering, hard impact.
For the small 3/4 x 1/2 job you're describing, I would just use a 3/8 or 1/4 carbide endmill.

[GJeff]

Always use the smallest endmill that can get the job done in a relatively fast manner.
Think about it.
If you swing your fist around at arm's length, it will make a hard impact.
If you hold your fist against your chest and swing around, it will barely make any impact at all.
Small diameter = less impact.
Large diameter = hammering, hard impact.
For the small 3/4 x 1/2 job you're describing, I would just use a 3/8 or 1/4 carbide endmill.

This is not right. You want rigidity, and the larger end mill you have the more rigidity. Always use the largest end mill you can and use the proper spindle speed combined with the radius to get the desired SFM.

A fly cutter might be like your fist swinging around, and you want it set to the smallest radius that works for the cut, but that doesn't apply to end mills.

[zero_divide]

Assuming 302 stainless:

4 flute cutter, 0.500" DOC, taking off 0.250" on each pass (only using half the cutter, overlapping passes, conventional milling), makes it 12 ipm, 1400 rpm. That gives you 0.9 hp required, 186 sfm, with chipload of 0.002" per tooth.

That is from FSWizard (FSWizard - Free Advanced CNC Speed and Feed Calculator). One of these days, I will buy a copy of GWizard.

Personally, I would probably cut the first pass at 0.250" DOC and see how it went, but than I am a wuss sometimes.

If you are not going to finish it with the fly cutter, than save 0.020" for a last finish pass with the end mill to clean it up.

Another solution is a face mill, assuming you have a small one (3/4" diameter). I dislike the interrupted cutting when hogging off material, but than I am in the business of maximizing tool life, not production.

Man, you are ruthless!

Using my free software and planning to buy competitors instead of my HSMAdvisor?
Sigh, i guess my "bait" strategy is not working

[SCzEngrgGroup]

Man, you are ruthless!

Using my free software and planning to buy competitors instead of my HSMAdvisor?
Sigh, i guess my "bait" strategy is not working

Eldar,

FWIW - I MUCH prefer HSMAdvisor to GWizard! I find I can nearly always just take the numbers it generates, and run with them, without even bothering to do test cuts, unless I'm really getting close to the limits of the machine. It is a GREAT tool!

Regards,
Ray L.

[tmarks11]

Using my free software and planning to buy competitors instead of my HSMAdvisor?

hmmm, er umm...

I guess I missed the stand-alone software link. I will have to check it out and do head-to-head with your competition. You should put a banner-add on the FSWizard page advertising...

If it makes you feel better, I do have the iOS FSWizardLite on my iPhone... oh, wait... that is free too, and I have not upgraded to pay you for FSWizardPro....

In my defense, most of my machining to date has been manual, and rpm=4*sfm/D & feed=RPM*T*CL is pretty easy to handle in my head...don't need to plan ahead like you do cnc.

[tmarks11]

You want rigidity, and the larger end mill you have the more rigidity....

+++1.

Also, the larger end mill does not really equate to significantly larger cutting surface, so Russ' analogy is bad. Think about how the end mill cuts: the curved edge of the cutting surface is doing the work. I suspect that the actual difference in exposed cutting edge length intersecting the work area is not significantly different. Smaller end mill is not really "concentrating" the force applied.

"Hammering" as Russ puts it only happens during an interrupted cut. A 4 flute cutter has at least half of the cutting edges engaged (assuming WOC of half the diameter), so no "hammering" occurs. If it sounds like your end mill is hammering when you are cutting, then you are doing something wrong.

Maybe Russ was talking about face mills? Those will hammer pretty good..

Large endmill: more rigidity, more room for chip clearance and larger WOC means larger chips that can carry away more heat, which means less heating of the end mill. The larger end mill has more thermal mass so less likely to over heat. Also can have a longer cutting edge for the same rigidity as the smaller end mill which means larger DOC (recommend DOC is usually about 2/3 of diameter).

And larger DOC = more heat carried away from the work piece.

The only reason to go to a small end mill is if the geometry of your cut put demands it.

Large end mill = larger WOC, Larger DOC - > Large chips, less heat, cutter lives longer
Small endmill = smaller WOC, smaller DOC -> Small chips, more heat, shorter life

[diyengineer]

Thanks for all the help. I'm going to try out that iphone app, sounds interesting!!

Goes to show paying attention to what your doing is most important! Don't let your girlfriend distract you like me haha. I'll order up the right insert also.


Washington state