Now I'm a believer; you can mill C1018 at 800 FPM

[tobyaxis]

Originally Posted by Geof But these also are insert cutters.

Are you saying that I am Off Topic Sir?

Yes they are. I will see if Hanita has a video of of the VariMill End Mill.

Did a quick search, no luck.

[Geof]

Originally Posted by tobyaxis Are you saying that I am Off Topic Sir?...

I'll let you get away with it because you called me 'Sir'.

Insert cutters behave very different to solid end mills and it is not difficult to drive them at very high speeds and feeds. They are generally bigger and can take bigger cuts which means the heat departs in the chip more effectively. Most of the videos I have seen of inserts cutters being driven show the cutter just ploughing straight through not doing the scalloping type cut that works with solid endmills.

[tobyaxis]

Originally Posted by Geof I'll let you get away with it because you called me 'Sir'. Insert cutters behave very different to solid end mills and it is not difficult to drive them at very high speeds and feeds. They are generally bigger and can take bigger cuts which means the heat departs in the chip more effectively. Most of the videos I have seen of inserts cutters being driven show the cutter just ploughing straight through not doing the scalloping type cut that works with solid endmills.

SIR (LOL)

Watch the Ingersoll Vids. There are some very nice Profile and Helical Cuts. All different alloys and cutting shapes.

[Donkey Hotey]

Ahh...OK...I didn't know we were excluding insert cutters. Nope, no solid ceramic endmills that I know of.

[tobyaxis]

Originally Posted by Donkey Hotey Ahh...OK...I didn't know we were excluding insert cutters. Nope, no solid ceramic endmills that I know of.

Maybe you should make one. Deal is that you will have to give everyone in this thread a free 1/2 3 flute.

Sound good??

[Matt@RFR]

Originally Posted by Geof But unless they have changed things you need to pre-drill at the center.

All you'd have to do is keep the code you allready have for the first helical ramp down the center of the bore, then position to the center of the bore, then start the G12/G13.

Might be faster to pre-drill anyway depending on how many holes are in a part versus tool change time.

[Geof]

Originally Posted by tobyaxis Maybe you should make one. Deal is that you will have to give everyone in this thread a free 1/2 3 flute. Sound good??

Just imagine if you could get ceramic cutters with the toughness of high speed steel.

[tobyaxis]

Originally Posted by Geof Just imagine if you could get ceramic cutters with the toughness of high speed steel.

With all the technology today that should be possible, right?

That would make for one hell of a tool. Speeds and Feeds would be limited only by your machine capabilities.

[Andre' B]

Originally Posted by Geof I did a helical ramp all the way through, came back to the top moved to a larger radius did the helical ramp again then back to the top for the final one. Yes an alternate method is to go through and spiral out and this spreads the wear on the cutter, but there is a problem. I am absolutely wonderful at hand coding but hand coding a spiral path could be something of a challenge. I have approximated a spiral by doing offset semicircles and increasing the radius on each one but even that involves a lot of coding when the radius increase is 0.025". Even coding sequential circles separated by radial moves out is a lot of work and the problem with this is that the radial move puts a big load on the cutter. And I am d****d if I am going to learn writing macros or CAM just for one fixture.

If you ever want to give it a go here is a bit of code that, starting with a 5/8 drilled hole, would spiral out then do a clean up and some spring passes. NCplot says about 30 seconds.

()
(OPEN UP BORE)
#33=0.025(SPIRAL PITCH)
#32=10.0(DEG PER STEP)
#30=0.060(START RADIUS)
#29=0.570(END RADIUS)
#27=-0.8(DEEP)
#26=110.0(FEED)
#25=1(SPRING PASSES)
(*****************)
(*****************)
(*****************)
#28=#30(SAVE START RAD)
#31=0.0(CURRENT ANGLE)
#33=[#33/[360/#32]]
G0X#28Y0.000
G0Z0.100
G1Z#27F#26
#31=#31+#32
#28=#28+#33
WHILE[#28LE#29]DO1
#1=#28*COS[#31]
#2=#28*SIN[#31]
G1X#1Y#2F#26
#31=#31+#32
#28=#28+#33
END1

#28=#31+[360*[#25+1]](FINISH PASSES)
#32=#32/4(MORE STEPS FOR FINISH)
WHILE[#31LE#28]DO1
#1=#29*COS[#31]
#2=#29*SIN[#31]
G1X#1Y#2F#26
#31=#31+#32
END1

G1X0.000Y0.000
G0Z0.100

Edit: Upload screen shot.

[Geof]

Originally Posted by Andre' B If you ever want to give it a go here is a bit of code.....

Thank you. I will try it some time although I have to check that Macros are activated on my home machine.

How long did it take to write that? I have done two simple macros and because I don't have all the stuff about what equals what memorized I spend a lot of time shuffling back and forth through pages in the manual looking things up.

[tobyaxis]

Originally Posted by Geof Thank you. I will try it some time although I have to check that Macros are activated on my home machine. How long did it take to write that? I have done two simple macros and because I don't have all the stuff about what equals what memorized I spend a lot of time shuffling back and forth through pages in the manual looking things up.

I have a PDF manual from a friend that works for HAAS. Would you like me to email it to you Geof? It isn't the greatest but it does give some reference to the assigned variables. Zipped it is 6.4mb and 12 unzipped.

LOL I will send it later because the WiFi network here is a little slow.

[Andre' B]

I think it was just an hour or two but it is one of those things where you just take some old program and modify it for the current need.

This is the version I use most of the time for a quick face cut on electrodes.

#112=1.200(FACE OFF SIZE)



()
(FACE OFF)
#33=0.200(SPIRAL PITCH)
#32=10.0(DEG PER STEP)
#31=0.0(CURRENT ANGLE)
(----)
#33=[#33/[360/#32]]
G0X#112Y0.000
G0Z0.500
G1Z0.000F40.0
#31=#31-#32
#112=#112-#33
WHILE[#112GE0]DO1
#30=#112*COS[#31]
#29=#112*SIN[#31]
G1X#30Y#29
#31=#31-#32
#112=#112-#33
END1
G01X0.000Y0.000
G01Z0.100

Been using MasterCAM more lately so have not been doing as much macro stuff. I do like the new high speed paths, the peel milling and core milling especially, hope they get some of the bugs worked out soon.