CNC Ø1/32" bit of choice.

DanO

DanO

AzB Silver Member
Silver Member
I’m setting up to cut some floating forearm points & I’m seeing an old friend again. I’m going .135” deep @ the base since I don’t have a Z offset to level the cue on my homegrown machine. I’m getting a nasty fishhook at the base point of my test pieces on my finish .003 pass. Doesn’t seem to matter CW or CCW. I get my best cutting performance running my machine @ 15 IPM roughing and 4 to 8 IPM finishing. I don’t see this problem on shallow pockets.

The max depth of cut on my Ø.031” carbide 3 flute mill is .165”. I think I’ll order some 3 flute .140” DOC to see if I get less cutter deflection into the deep pocket corner. Or I could try a 2 flute .130 DOC even though I’m cutting .135 deep. Dick mentioned quite a few coons ages ago that the curf makes a nice lead in.

From earlier conversations I believe I’m using the best cutter supplier out there, I’m just thinking I may not be using the right tool for the job?
 
Try inserting a pause command (G4 P?) into the G code.
Even a .5 sec delay has help to save tools from breaking,
allowing the tool to relax. Know tool breakage is not the
problem here, but sometimes anything will help.

Bob A
 
Dano,

I am no expert but I do a lot of pockets at .120 with a .0313 2 fluke using a 50% cutter encroachment doing conventional milling. I cut at 5 to 8 ipm with a .004 clean up pass with only 2 Z elevation cuts, .060 & .120. Ebony or ivory being at 5 and maple being at 8.

I know a lot of guys go 18 and do multiple depths and I have tried that. I seem to get better results with 2 depth cuts that are slower. On geometry that has arcs I always put the arc slow down at 50% as a rule and it does a nice job.

Rick
 
In general machining theory 2 times the diameter is considered a DEEP cut, and so should be compensated for either in less stepover, and/or feeds and speeds. Recutting chips hurts cutter performance also and so get them out of the cavity with either vacuum or forced air. Forced air is generally preferred because it helps keep heat away. Also, use less SFPM in denser materials.
 
I'm cleaning the pocket with air as i cut. My step over is 50%. I have my arc speed set to 75%. I'll try 50. Rick are you doing two clean up passes @ .06 deep or just 1 @ .12? The final pass is what's causing me problems. I may try to dub a program cutting the final clean up in 2 passes. The included angle of the pocket giving me problems is 40º.
 
Hey Rick, I like your clean up @ half the full depth rather than the full .120. Your'e not cutting the full .06 depth in one increment are you? Even @ 50% overlap the seems excessive.

So you prefer the 2 flute cutters over the 3?
 
Hi Dan
at that depth of cut and those speeds i dont think you will ever get a fair evaluation of the endmills performance. By the time you get to your cleanup pass it is probably quite hot and possibly dull.

Are you out in the middle of the cue, when this is taking place? A big cutter like that "especially a dull one" will push the cue around where it is unsupported. Might be intensified with dull cutter and abrupt moves out of sharp corners.

Just some food for thought.
 
cnc

Thanks for the info.
Just a few things to think about. There is a lot of over hang on the spindle.
Looks like it's a long way from the mount to the tip of the bit. Lends it self
to deflection. With 3 flutes, you have to move that baby pretty fast or as has been said, it will get hot. I don't see a steady rest in the middle of the cue. If you get pushing that much material, it's amazing what kind of deflection you can get. Then as the feed rate slows down you get inconsistant tool paths. For cues, I really like 2 flute cutters.
I'm definitely not an cnc expert, but I would give a try at hogging with a
larger endmill and then going back in and cleaning up with your final size, but
leave more meat for the clean up pass. Say more like 8 or 10 thou. And definitely make it a climb pass with the highest speed rate your machine can handle. Nice machine by the way, it should be able to handle some good speeds. I've accidentally ran a.0312 cutter in excess of 50ipm, .120 depth of cut and not broken it . And that was thru high density particle board.
 
Very good info guys. Thanks for all the help. I've made an upgrade to my Z axis since that original post. I added a secondary slave slide to help reduce the deflection over the length.

Based off what I'm seeing and now reading, I think I'll make a steady rest with a center bearing. Thinking back at when I originally had this problem in another cue, I did not get the fishhook on a nicely clamped test board, but I did when I cut the design in the cue. Next, I'm going to order some 2 flute cutters with a shorter DOC today. Last, I'm going to cut and paste my finish pass into 2 depths, reduce my curve speed to 50%, and maybe add a dwell but only if I have to since I'm not certain how to do that.

Thanks again.
 
Cnc

Please let us know how it works out, and what you finally determine
was the root problem.
 
DanO said:
Very good info guys. Thanks for all the help. I've made an upgrade to my Z axis since that original post. I added a secondary slave slide to help reduce the deflection over the length.

Based off what I'm seeing and now reading, I think I'll make a steady rest with a center bearing. Thinking back at when I originally had this problem in another cue, I did not get the fishhook on a nicely clamped test board, but I did when I cut the design in the cue. Next, I'm going to order some 2 flute cutters with a shorter DOC today. Last, I'm going to cut and paste my finish pass into 2 depths, reduce my curve speed to 50%, and maybe add a dwell but only if I have to since I'm not certain how to do that.

Thanks again.
Click to expand...

You should be able to just program your tool path at a single depth, as a sub program, and then peck with it at incremental steps for pecking. This keeps the program shorter.
 
I believe the largest culprit to my problem was the lack of support on the cue. I went with a larger 5C collet and choked up on the bat.

The second culprit was the depth of my finish cut. I broke the program into to finish passes. Now the cutter sounds no different in the corners as it does in the flats.

Last, I went with a 2 flute end mill with only a 1/8” max depth. Now it looks like I can tighten up my .002” per side offset. I’ll have to play with that next.

Thanks guys. Sometimes the simplest of changes are the most logical yet hardest to see. For me anyway.
 

Attachments

  • 120716-4.jpg
    120716-4.jpg
    82.2 KB · Views: 172
You must log in or register to reply here.
Back
Top