LinkBack URL
About LinkBacks
tried 60ipm @2500rpm with a .030" step over. It ran well for 75% of the cut, until the tool dulled, and it moved in the collet?? Gonna see if the solid holder helps.
| | |
I have a 4.5" wide x 20" long 1" thick AR-400 plates that need a centered slot cut completely through them 3.0625" wide by half inch deep. I have some 5/8" solid carbide endmills that i would like to try a trochodial tool path with, basically just for practice and to test this kind of tool path. I only have a few to make and no time restraints, so this is a good one to learn a bit on. I am wondering what kind of step over i should run, and rpm and chip load?? I know what i would do for mild steel, but am a bit stumped on this quench tempered stuff. I realize this is more of a face mill operation, but just trying something different while I'm learning MasterCAM
tried 60ipm @2500rpm with a .030" step over. It ran well for 75% of the cut, until the tool dulled, and it moved in the collet?? Gonna see if the solid holder helps.
what brand carbide? coated or uncoated?
what type collet holder?
I am assuming you have a real machine? if you dont more than likely the spindle is sloppy and the vibration wore the tool down.
kennemetal Harvii HPHV KC633m has a bullnose of .030 too
Ya its a real machine 25hp spindle 78"x33" table has a weight of 15000 lbs +, but i was only running an ER40 collet (i know, i know, but all i have at the moment besides a 6" solid weld-on holder)).
are you getting alot of vibration using the er-40?
BTW I tried the trochodial tool path over the weekend 1st time as well.
with a garr 3/8" 4 flute endmill 2" length of flute to rough out a tree pan. I found I had to slow my feed up 50% .250 DOC. put alot of wear on the endmill too.
Delw
For what it's worth I think your speed is a bit slow, your step over is too much and your feed is too slow. But I don't often machine anything with a tensile five times that of 1018 with high abrasion resistance as well so maybe I am too optimistic.
I do think you need a TiAlN coated cutter running dry with a strong airblast and even if I did not increase the speed I would drop the step over down to something like 0.01 and take the feed up by 3x. The idea with trochoidal is to get a thin, hot chip that activates the coating and is moving past the tool fast so there is not enough time for the heat to transfer to the tool or conduct back into the work piece. Also for this application I would not use a bullnose because the chip flow around that radius is not nice and smooth.
An open mind is a virtue...so long as all the common sense has not leaked out.
Thanks Geof, I didnt know that.Originally Posted by Geof
I got some coated ones coming tomorrow. I will speed mine up and thin out the cut thickness and depth.
not much vibration at all until the tool began to wear. I will try again down the road with some 1018 and see what happens, I just went back to the face mill, and this stuff is still a pain to machine. It is extremely tough and hard.
What do you guys use for entrance and exit radii? a percentage of the tool dia.? i put in .5 for a 5/8 cutter and it seemed to be doing a lot of "air cutting"
I ran another part just about 20 mins ago 3/8 garr coated end mill 20ipm 3000rpms, .250DOC
xy step over
min .090
max.168
2º plunge angle 30% initial rad.(.1125) and 50% retry loop with a min loop of 3%
I used the area mill havent tried peel mill havent tried peel mill yet.
I did use flood coolant ( was chicken not to).
the program was quite large so had to dnc it at 9600 baud rate
I think I can feed it up if I drop the xy step over
the material was 4340 at 38-40rc If I remember correctly( dont have the certs in front of me)
My first try in the above post with the 2" endmill was like at 5ipm and 1200 rpms using standard carbide.
this time I tried a regular length endmill coated for high speeds.
chips were big but looked good and make it through .750 DOC with no problems.
I am just removing some material for a treepan I have to do.
its a pretty cool programing technique, I have some jobs coming up I can definately use it in and going to try 5 fluters for it..
The mill I was running this in was a max 1 rebel 1997 with a fanuc o-m control, I use it for tooling and easy stuff or just playing.
Now I want to try this will Alum on some thin grooves that I use 1/16 and 3/32 endmills on , I think it could speed up production alot in the haas.
Delw
I was using the peel mill when i did it, as the part had an open entrance and exit. There is a lot less options listed here then the area mill, which i haven't used yet but played with. We did do a contour path from a sqaure to a profile on the inside contour, using .030 depth of cut and an .008" load at 5000rpm with a 1/2" cutter, as a demo. That was something to see. Chips were 6-8' in the air. It kinda of used the same principles, really light but fast cuts.
Posting Permissions
| | |
