Tooling failure profile cutting nested parts

[dingo0722]

I am working on cutting out parts from a 5x12x 5/16 sheet of 304 stainless. I am able to nest 11 parts into the material and perform all the drilling operations with out problem. I run into issues when I go to cut out the part from the stock. I seem to keep breaking endmills when cutting out the part. I have tried different sizes and found 0.25 carbide 4 flute works but need to reduce the nested quantity. Since I al cutting with the full diameter of the endmill does anyone have any recommendations at to what type of endmill would work best and the speeds, feeds and depth of cut I can run this at. Right now the profile run time is about 30 minuets.

See attached picture

thanks

Dan

[neilw20]

What depth of cut using the 0.25 end mill.?
Are you plunging down or ramping?
What feed rate have you tried.
Are you using coolant?
How do you stop the finished part moving as it breaks free?
Do you screw them down? You have holes on fished parts to do that.

I have found that if one tip on a 4 flute gets damaged the other 3 overload and fail soon after as the tooth on the other side loads up the chipped tooth.
Using a 3 flute cutter, each tooth is independent and does not have a tooth on the 'other side' so if one chips it just seems to soldier on.

[dingo0722]

I am plunging down. Using a 0.25 center cut endmill I plunge 0.015inches. I have a rpm of 2500 and feed of 8ipm. I am using a mist coolant system. I have found the carbides to be extremely unforgiving here. Should I consider a coated HSS 3 flute instead.

To prevent the part from moving I have been leaving between 0.005 to 0.01" on the bottom. I have had problems with repeatability there since all our stock was sheared and has a slight camber in it. I was thinking of making a jig to hold the part in place during the operation and using a fastener to hold each piece during cutting

[neilw20]

I have had more success with uncoated.
The extra expense of the coated make for very accurate cutters, but once there is the slightest damage to them the underlying surface is a different hardness.

I am using uncoated 3 flute cutters on stainless and have found they normally come supplied with 8 degree clearance on the cutting face.
It take very little wear to end up with a flat on them, then they rub and the cutting pressure increases. If the front edge of the cutter has the helix angle as clearance it is much weaker, so I put front clearance of 5 degrees just down the flute a little.

I regrind them to 5 degrees and a 2 degree cone angle and they last twice as long.
[nomedia="http://www.youtube.com/watch?v=lzCeAsDMCR8"]YouTube- SNC00374.mp4[/nomedia]

I use an even faster setup now. Under 2 minutes per cutter, dry.

I am cutting fiberglass on stainless substrate, and once I have a 0.1mm (0.004") on the tip they are useless for my job.
With coated cutter, they were very accurate, but lasted maybe 20% compared to the uncoated.

I have 33 of them I use on one job. They last me 1 hour each.

I found 1400 RPM best for a 10mm which means about 2200 for 1/4".
I am using them dry, so increasing that by 50% would seem OK.

2500 and 8IPM sounds OK. but with a 3 flute you would drop that to 6IPM

When you machine around the edges do you use the full depth.
I think you need to do it in three passes, and would ramp down from 0.015 and make it so that you get to the full depth after three times around the part.

It will be almost all the way around the part before it breaks through so you could get away with 1 holding screw near the end of the cut.

Climb milling by going clockwise around your parts will give better tool life and a nicer finish.

I never side cut DOC more than the cutter radius.
Don't they make awful splinters!!!

[dingo0722]

So this is what I will try out.

1/4" 3 flute uncoated HSS running at 2400 RPM and 6 IPM with a depth of cut 0.104" making 3 passes. I will ramp down to each cut level. I am also going to secure the part onto a consumable board so I can secure each piece.

This should be interesting. But considering the # of carbide endmills I have eaten making 30 pieces Im open to anything. I have had great luck with HSS and Cobalt drills making this part.

Ill keep you updated. Cutting some H13 now, renews my confidence I can machine parts :-)

-Dan

[neilw20]

Myself, I would ramp down all the way, spiraling down.
After the first time around you are at max depth of cut and the cutter load stays constant, and at the end keep ramping down into the sacrificial board allowing more even wear on the flutes.

With a reasonably constant cutter load deflection does not change rapidly, as it would change as you do a short ramp down to the next level. Even ramping from just above zero into the job will save the cutter from initial damage. The initial ramp can be a bit more aggressive, decreasing the feed once engaged and stable.
The very long ramp angle will stop excessive load on the trailing edge of the cut. Near the end of the cut increase the feed a bit so that the load stays more constant as you are breaking through.

Hand coded, this is easy, but with a CAM program will be a bit of a challenge, unless it is a really swish program.
I let the cam program generate the tool X,Y path then hand code the ramping. Machinists are often more savvy than the best of CAM software writers.
Only the ones who make the chips have the experience. (IMHO) Someone prove me wrong.

Tell us how it goes.

Fine tuning seems to make or break some jobs.
I have been doing a particular job for 20 months now, and the fine tuning has tripled the cutter life, and decreased cycle time even now.

It is working so well now, my wife runs the SX3, which is stabilized to a brick wall.
The brick wall increased Z accuracy holding capabilities at least 20 fold. At tool change, Z is within 0.005mm. SX3 rocks!