Pocketing, any tips??

[jspangler]

Hi

I am new to MC and CNC machining and have been doing OK, but am wondering if i can't speed things up a little here. First question=

What tools, speeds and feeds, and depths of cut do you recommend when pocketing .375 thick 1018. I am making header flanges so most of the pockets are no bigger than 1.75 x 1.75. I've been using Iscar insertable 1" end mills and the 328 inserts, so far. Everything is held down tight. Second question, is it possible to dril the heck out of the pocket to eliminate as much material first then run a clean up with the mill on the outer boundary, or will the loose material beat up the tool too much?

Thanks

John

Hotshot Performance, Inc.

[jspangler]

Oh Yeah,

I am using a Haas VF-2, the shortest tool holders I can find, and running coolant.

 

I think that's it.

 

Thanks

John

Hotshot Performance, Inc.

[Keith Graydon]

Hi,

Is this header flange really a pocket (blind area) or is it a window (thru area)? When I think of header pipes I think that the flange is a window. If that's the case then DONT pocket it. Just Contour it. much less time to cut. Watch out for loose slugs 'tho.

The old adage about speeds and feeds for steel is:

quote:

---

RUN IT TILL IT TURNS BLUE

---

Hehe. just check with the insert maker for recommendations or program it in Mcam using "feeds and speeds" from material. Do this from "JOB SET-UP" dialog.

 

HTH

-KLG

[jspangler]

Hi

That's what i've been doing so far for speeds and feeds, but depending on the depth of cut (obviously never more than .375) on an apkt insert, the machine sounds like it's about to fall apart. This is with a really secure fixture, short holder, etc. I'm using the constant overlap pocket method from the center out, with 40% overlap. I'd like to be able to do it in one pass....

Is there a way to make the cutter know that in a 1.5 dia. pocket, and that i've drilled a 1" starting hole, that the .75 end mill will start cutting right away and not spin in the center a bunch before cutting???

 

Thanks

John

[Guest CNC Apps Guy 1]

Hello John,

My personal preference when cutting steel when using inserted cutters is to run it dry. This will tell you where you are SFM-wise. In ideal work holding conditions you'll probably want to be in the 500-800 SFM range if memory serves me correctly. As was stated earlier, the chips should be blue when machining with Inserts.

If you need any other help John, don't hesitate to ask.

[JAMMAN]

I'ts been a LONG time since metals for me but I have to support James in his "run it dry" belief.

Crank the feed till the chips turn blue, blow them out of the way with air.I did that with not only insert tooling but solid carbide cutters also.

[McRae]

When pocketing, remember that the perifery of the cutter will be at a higher "Linear" feedrate when interpolating around a corner and so you should compensate for the internal arc feedrate. The Iscar 328 is a stable grade but I would use the 950 as it is more wear resistent and will allow you to run with a higher spindle speed. (For 1018 plate, I would go 800-1200sfm and a fpt of .006)

Use an AIR BLOW to get the chips out of the way - Recutting chips is asking for trouble.

For the 3 flute cutter in question with the APKT 15mm insert, RPM=3000 FEED~54ipm. Ramp down at 3 degrees and use a .3 factor for ramp feed. Watch the feed in the corners and slow down using a factor that relates tool diameter to radius interpolated. If the machine still hammers, try reducing the number of flutes to two (another cutter) and increasing the feed per tooth to .008/.012. ***Run Dry*** when the chips are first off the part they should be shiny silver. Don't touch them but watch as they begin to turn blue as they cool. If you use coolant the insert will micro fracture along the cutting edge and premature failure will result. Watch the load meter on the machine with a fresh set of inserts. Tool life is over when the load meter goes 30% over this (my personal limit, others may go as much as 50% but I have a limited steel budget!).

Maximum profit lies just below the safety limit - so use caution!

MfgEng

[jspangler]

Hi

thanks for all the tips.

One more question though, when you mention adjusting the feedrateon the arcs, is there a way MC does this automatically without adding too much time to the cycle, or is it something you do manually when you post?

 

Thanks Again

John

Hotshot Performance, Inc.

[Scott Bond]

Hi

keithgraydon wrote

"If that's the case then DON'T pocket it. Just Contour it. much less time to cut. Watch out for loose slugs 'tho."

This is what I did with a forty taper,that wasn't rigid enough for larger dia. tools.

I used this method on a triangular flange that had three bolt holes -and one large hole in the middle.

Simple fixture ,a plate with toe clamps .

Drill the three bolt holes one in large hole and one entry.

M0 ,add four bolts.

Use 3/8 rougher .(smaller dia. has less torque)

I used a high pressure coolant to blow the chips off.

Finish with four flute finisher.Because it only removes .005 it will last a while

[Hugh.Venables]

John, have a look at "Compensating feed rates on arc moves" on page 2 of this forum. A few suggestions were made. Northwood Designs will send you a very well written paper explaining the wonders of their Meta-cut Finish product. Sounds excellent. Their 30 day trial is a snail-mailout that costs although I think there is a link on their website to a free on-line demo at another site. Ask for the full price too.

You can manually calculate feedrate corrections by multiplying your specified feedrate by (1-C/J) for internal radius and by (1+C/J) for external, where C is the cutter and J is the job, both in radius or both in diameter. Editing after posting is pretty tedious and we're using MCam to avoid that, aren't we.

Hugh Venables.

[jspangler]

Hi

That's what I thought...

How does MC's High Speed machining compare to these programs. I tried to DL the Metacut but the free demo didn't work. Would High Speed Machining help in my specific application, since it's the only thing I currently use the machine for??

Thanks

John

Hotshot Performance, Inc.

[MasterNick]

Hi John, i just wanted to let you know that I'm using a Haas VF3 and in the settings, setting #44 there's an option for a - min F(feed) in radius cc %:

I'm unsure if the VF2's have that option though, check it out.

[dsharpe]

I'd have to agree with Scott Bond .A 1" inserted cutter in steel on a light 40 taper M/C is pushing it. I'd go for a small carbide rippa cutter - iscar sells them - probably just as quick and much easier on the M/C.

Dave