Dynamic mill

[Matt Boozer from L&R PT]

Has anybody tried to us this in a 3 inch deep pocket?

 

I have a pocket that has a raduis of 5.5 inches at one end and a raduis of 4. inches on the other,the center are 6.25 apart, then the arcs are joint by tangent from on to the other. The material is 1045 hot roll.

 

I haven't ran this yeah but my question is were do the speed and feed come from, I suppose maybe you would call the tool manufacture? Any other insight would be great.

[Tony35]

i have done it in a 2in deep pocket that was thru in D2

 

i was using a varimill coated 500 SFM .03 stepover @ 83 IPM with air blast seem to cut very well

 

how big of a tool are you going to be using?

how much HP does the machine have?

rigid setup tool/part?

tight machine?

[Matt Boozer from L&R PT]

Tony,

 

What kinda times did you get with that set-up?

 

The machine is a Haas VF3. I do have 300 psi thru the tool. I'm using 2 6" kurt vises with the part sitting all the way down in the bottom.

 

I have plunged milled it and the part didn't move at all. The problem with the plunge mill with the iscar tool manufacter rep. standing right there giving the speed and feed recommendations didn't save me any time from using the 1 1/4 hogmill( 2 hours). The plunge tool was 1 1/2 and it took 2 1/2 hours to rough out.

 

I just had the mitsubishi rep here and he gave me a tool to try and that worked really well

(1 hour 10 minutes)use there AJX line of insert tools.

[Tony35]

it was a 5 X 6 inch pocket with 2.0 rads in the corners 3/4 solid carbide varimill with air blast took about 7-8 min to rough it out kitamura 4XiF VMC 50 taper 25HP spindle

 

with side milling you get great tool life/wear so with a small stepover you can apply chip thinning to the cut and get more feed out of the tool i only had 1 tool at the time so i didnt push it but it could of taken more feed

 

you could do it in 2 depth cuts of 1.5 or the full 3 if the tool/spindle will take it i think it might be faster have you programmed it in dynamic mill just to get a time of how long it will take vs what time you have now

[Ron Branch @ Verisurf]

Well with a Seco 2" highfeed cutter I would run it at these speeds and feeds. 2000rpms at about 300 imp and .055 D.O.C and tell me how fast that cuts out that pocket.

 

HTH

[[email protected]]

++1 Ron to the high feed cutters

 

I cut an odd shaped pocket 1.968 deep and if you squared the pocket it would be 13.5 x 13.5 using Iscar 50mm Feedmill 1990 rpm @ 308 ipm @ 1mm doc

and it took around 38 minutes

 

I'm sold on highfeed cutters

[Leigh @ Kodiak]

+++ on the high feed cutters. Off the top of my head, I would guess you could rough out that pocket in 30 -40 minutes with a high feed cutter.

[Tony35]

i tried high feed cutters on the parts we do and no dice

 

setup not rigid enough and tool was hanging out to far to get the depth i needed plus they dont like to break thru on thru pockets

 

i wish we had more parts that i could apply that tool too but oh well

[Leigh @ Kodiak]

I ran a 1.5" dia. feedmill that was 8" long. I also broke through the floor. The key is that as your cutter gets longer, reduce the DOC, but keep the same feed rates.

[Matt Boozer from L&R PT]

Right now I'm using the mitsubishi AJX high feed and running 114 ipm and speed of 1867 with a time of 1 hour 10 minutes.Just using a a standard pocketing toolpath.

 

I also had our mastercam rep here to and we played around with the dynamic milling and smoked a 1" endmill.

[Leigh @ Kodiak]

what DOC are you using? Cutter dia?

[Matt Boozer from L&R PT]

I'm going a Doc of .031 and 1.125 cutter.

 

I know that sound small but I'm using that cutter to rough in some deep counterbores too.

[Leigh @ Kodiak]

Seems like your FPT is a little on the low side. If you are wary of bumping it up, just try making your DOC deeper. Only go .002 or .003 deeper at a time.

 

It doesn't seem like much, but over only a 1" deep pocket, .003" extra DOC means 2 less passes to get to depth.

[Gary]

Gunguy, you are right in the feed/rpm I have to run our haas at on 4141ph. I have seen bigger machines blow it away but that's wear the haas likes to run. You should be able to walk away from the machine and have about 3hrs insert life with what your doing. I like the unattended running at not killing the machine myself. In soft stock you should be able to run in the 150.180 feed range, but I use highspeed paths so the step over is smoother.

[cadcam]

So any one playing with 304 ss I am just starting and see what I can get from it.

 

I did do some pockets with a 3/16 SGS Zcarb 4flt.

.25 DOC and 15% axle cut helix in at 12 IPM and cut at depth at 46 IPM and saw only 6% spindle load and cut great. I am going to try more and move fast I feel this for the 304 SS is going to be a great tool.

 

Same result in another pocket but i drilled first for 304 ss .5 DOC with a 5/16 3flt carbide rougher at 42 IPM.

 

I feel these are low to what i think can be done with this tool.