High Feed Mills and Conventional/Climb Cutting

[mackenzieruiter]

I have spent around 2 hours today digging through forums all over and I haven't found a decent thread on this subject.

Reason I bring it up and ask is because I have heard this through word of mouth and now from my Tool Rep.

So, what is the general consensus on this? Climb only? Zigzag? Conventional only on entry? 

[kyle528]

If high radial DOC and small axial, I like to zig zag, if high axial and lower radial (think HEM style milling) I like climb only

[Jobnt]

Based on my own personal experience I usually climb-only on hard metals and will zig zag the hell out of soft stuff like alum and plastics.

[sweeden5050]

Typically I will zig zag on softer materials. When harder material I always climb cut. 

[Tim Johnson]

We make some 303 stainless heat sinks and we slot the fins in with a 1/8" high feed mill. We run it at 15000 rpm at 335 ipm. If our doc is more than .005" we will get early breakage. I'm verifying one right now.

[Jobnt]

^^^ Old-School HSM FTMFW!!

 

[jpatry]

On 7/22/2023 at 3:32 PM, mackenzieruiter said:

I have spent around 2 hours today digging through forums all over and I haven't found a decent thread on this subject.

Reason I bring it up and ask is because I have heard this through word of mouth and now from my Tool Rep.

So, what is the general consensus on this? Climb only? Zigzag? Conventional only on entry? 

Well, I just always use climb, mostly out of ingrained habit.

But I've been thinking that with the shallow DOC and over 50% stepover of highfeed machining the conditions that benefit climb vs conventional are not really present, so why not  go both ways and truly maximize cutting time.

[crazy^millman]

On 7/22/2023 at 12:32 PM, mackenzieruiter said:

I have spent around 2 hours today digging through forums all over and I haven't found a decent thread on this subject.

Reason I bring it up and ask is because I have heard this through word of mouth and now from my Tool Rep.

So, what is the general consensus on this? Climb only? Zigzag? Conventional only on entry? 

Such a deep subject to think about that I think others have touched on the different things to consider. Testing and seeing where the best ROI gives is what really needs to be done.

[huskermcdoogle]

On 8/14/2023 at 12:21 PM, crazy^millman said:

Testing and seeing where the best ROI gives is what really needs to be done.

DING DING DING

When running high feed cutters, in my experience, when climb should have worked best, conventional cutting has worked better, as well as the opposite case.  It is highly dependent on toolpath style as well as material and part shape.  When running in Ti, Inco, or other super alloys, I now always advise my customers to try both ways.  I have seen 3-5x differences in tool life with zero difference in processing time or speeds and feeds.  When you get that much more life often I have been able to really boost productivity by then balancing the tool life with speed and hitting the right tool change interval.  Let's just say you get 1 part going climb, you switch to conventional and you get 5 parts.  You then increase the speed 30%, and now you get 2.5 parts.  So you bump it up 5% more and now you get 2.1 parts and change them at 2 so you have a little wiggle room.  35% on productivity is huge and think, you are using 50% of the inserts you were.  It's a made up example, but to Ron's point.  TEST TEST TEST, you won't know unless you try.

[byte]

^ This guys gets it!

[mackenzieruiter]

On 8/13/2023 at 5:46 AM, jpatry said:

Well, I just always use climb, mostly out of ingrained habit.

But I've been thinking that with the shallow DOC and over 50% stepover of highfeed machining the conditions that benefit climb vs conventional are not really present, so why not  go both ways and truly maximize cutting time.

I am wondering if that is what my Walter Rep. was getting at.

 

On 8/14/2023 at 12:21 PM, crazy^millman said:

Such a deep subject to think about that I think others have touched on the different things to consider. Testing and seeing where the best ROI gives is what really needs to be done.

Then a test shall be done! I owe everyone at least something for the help I have received.

Should be able to get a few different scenarios put together with some different materials.

 

 

[Kyle F]

20 hours ago, mackenzieruiter said:

Then a test shall be done! I owe everyone at least something for the help I have received.

Should be able to get a few different scenarios put together with some different materials.

 

keep us posted on your findings 

[jpatry]

On 4/1/2024 at 11:46 AM, mackenzieruiter said:

I am wondering if that is what my Walter Rep. was getting at.

 

Then a test shall be done! I owe everyone at least something for the help I have received.

Should be able to get a few different scenarios put together with some different materials.

 

 

As always, the proof is in the pudding.

[jstell]

On 8/10/2023 at 9:26 AM, Tim Johnson said:

We make some 303 stainless heat sinks and we slot the fins in with a 1/8" high feed mill. We run it at 15000 rpm at 335 ipm. If our doc is more than .005" we will get early breakage. I'm verifying one right now.

I of course have no idea how far your tool is sticking out, but with a standard issue (coated, SS-cutting geom) 4 flute 1/4" l.o.c. 1/8" EM and flood coolant in 303 if i use the relatively (extremely this decade it seems) conservative sfm of 245 I get 7500 rpm and can get reasonable tool life (it's a $15 tool) at 24 ipm full slot width of cutter with flood coolant at .08 d.o.c. which seems really slow compared to your 335 ipm.  But when multiplied by d.o.c. it's actually a 15% faster volumetric removal rate.  And if I sacrifice a little tool life I can feed 10% faster or .09 d.o.c. which is 25-30% faster material removal rate than what you've got at .005 d.o.c.

But again, if you have 1/2" l.o.c. or a longer reach tool the depth and feedrate go down and you get the win with high-feed shallow d.o.c.

[Tim Johnson]

22 hours ago, jstell said:

I of course have no idea how far your tool is sticking out, but with a standard issue (coated, SS-cutting geom) 4 flute 1/4" l.o.c. 1/8" EM and flood coolant in 303 if i use the relatively (extremely this decade it seems) conservative sfm of 245 I get 7500 rpm and can get reasonable tool life (it's a $15 tool) at 24 ipm full slot width of cutter with flood coolant at .08 d.o.c. which seems really slow compared to your 335 ipm.  But when multiplied by d.o.c. it's actually a 15% faster volumetric removal rate.  And if I sacrifice a little tool life I can feed 10% faster or .09 d.o.c. which is 25-30% faster material removal rate than what you've got at .005 d.o.c.

But again, if you have 1/2" l.o.c. or a longer reach tool the depth and feedrate go down and you get the win with high-feed shallow d.o.c.

The cutter we use for the stainless heatsinks is a Mitsubishi VC-HFRB D1/8N5DR0.03. The flute is about 1/8" long and has a reach of about .650". I can't imagine a standard $15 1/8" end mill doing what this cutter does. I would think if it got through 1/4 of a part it did a good job. My guess is this little cutter is closer to $100. and very well worth it. We typically run 8 parts in one cycle and switch our cutter after each. We also use 1 micron coolant bags to collect the fines.

[Kyle F]

On 5/30/2024 at 11:25 AM, jstell said:

I of course have no idea how far your tool is sticking out, but with a standard issue (coated, SS-cutting geom) 4 flute 1/4" l.o.c. 1/8" EM and flood coolant in 303 if i use the relatively (extremely this decade it seems) conservative sfm of 245 I get 7500 rpm and can get reasonable tool life (it's a $15 tool) at 24 ipm full slot width of cutter with flood coolant at .08 d.o.c. which seems really slow compared to your 335 ipm.  But when multiplied by d.o.c. it's actually a 15% faster volumetric removal rate.  And if I sacrifice a little tool life I can feed 10% faster or .09 d.o.c. which is 25-30% faster material removal rate than what you've got at .005 d.o.c.

But again, if you have 1/2" l.o.c. or a longer reach tool the depth and feedrate go down and you get the win with high-feed shallow d.o.c.

the small dia high feed mills are quite expensive, so if you're trying to slot a shallow groove with them it's possible it could not be the best choice.

They really, truly shine at 5x diameter and longer stickouts/reach. I used a helical .125 high feed mill to rough a .14 wide, 1.2ish diameter groove. .125 high feed mill was something like 8-10krpm @ 100inches per minute, all the way to over 1.0" deep. (with no TSC) The ramp angle of course was very light something like .003-.005 depth per rev but I got through the whole batch of 316 stainless parts without changing that tool. 

So even if it takes longer, or is a bit costlier,.. I'll take the reliability all day--(and now on a matsuura, into the night)