Roughing, Climb only or both ways?

[Chips Everywhere]

This may be a silly question to those who run large production runs, as the answer may be very obvious, but as I start getting into the 4 digit production numbers I find myself trying to improve/reduce my roughing cycle times, wasted motion and improve my programming.

Material: Aluminium 6061-T6

Currently, I am roughing with a Helical # 82744 end mill (1/2" Diameter, 3 Flute, 0.06" CR, 2" LOC w chip breakers). I'm running it at 12k rpm @ 324imp, 1.75" axial and 0.075" radial engagement, climb mill only. One thing to note, I can't go over the end mill diameter I am currently using, as its the only size that will cut the features in my part.

My questions regarding production roughing are:

Can I run the end mill both ways, climb and conventional, to remove more material?
How does this play into tool life/ tool reliability?
Does one reduce speed or the radial depth of cut during conventional if both ways is selected?

I am planning on switching over to corncob rougher after I consume these end mills, as it seems you can get better material removal with them.

Thanks in advance

 

[plastikdreams]

I cut 2024 both ways, in 6061 you have to watch for bue especially on the conventional cut. As long as you can flood enough you should be fine. A corncob should rip the hell out of it though.

 

[Chips Everywhere]

I cut 2024 both ways, in 6061 you have to watch for bue especially on the conventional cut. As long as you can flood enough you should be fine. A corncob should rip the hell out of it though.

Do you maintain same depth of cut and feed when doing both ways? What is bue? build up on the end mill? I do have flood coolant

 

[mhajicek]

Do you maintain same depth of cut and feed when doing both ways? What is bue? build up on the end mill? I do have flood coolant

Yes, BUE is built up edge, workpiece material sticking to the cutter edge.

 

[rklopp]

Yes BUE = built up edge. Oops late on the draw.

 

[sinha]

Conventional milling starts with some rubbing before it gets into the biting point. This may have some impact on the tool life. Experienced machinists may comment.

 

[TAIWA NUMBA WAAN]

I have done both ways HSM'ing on some bigger aluminum parts. It works, but if your coolant stutters there is a real risk the endmill welds on the conventional cut pass, especially if you're taking a higher radial stepover.

If your coolant is reliable and you're using a roughing/corn cob endmill, both ways HSM will definitely outperform one way cutting in cycle time, by a lot.

 

[Speedie]

Always both ways in softer material

 

[CarbideBob]

6061.
If the machine with decent rapids I would be climb cut only.
.075 radial on a 1/2 inch tooling Al? Why?

 

[crossthread82]

Can you not rough with a 3/4 then finish/re-machine with a 1/2?

Usually when I two way rough I turn the conventional feed down to about 80% of the climb feedrate.

Good coolant flow is critical, if you have tsc I'd run it with a coolant collet so you have coolant blowing down the shank of the tool. Coated endmills also help out a bunch too, my flavor of choice is DLC or TiB2.

 

[Larry Dickman]

I've had no trouble roughing both ways (zig zag) with 1/2 or 3/8 cutters. With 3/4 or 1" cutters, I tend to get screeching on the con cut.

 

[Chips Everywhere]

6061.
If the machine with decent rapids I would be climb cut only.
.075 radial on a 1/2 inch tooling Al? Why?

It’s a VF2SS, so it’s ok rapids.

I don’t understand your second question or statement, are you implying that it’s conservative engagement or too much?

 

[Chips Everywhere]

Can you not rough with a 3/4 then finish/re-machine with a 1/2?

Usually when I two way rough I turn the conventional feed down to about 80% of the climb feedrate.

Good coolant flow is critical, if you have tsc I'd run it with a coolant collet so you have coolant blowing down the shank of the tool. Coated endmills also help out a bunch too, my flavor of choice is DLC or TiB2.

I tried that approach, and the part has too many hard to reach spots that it’s not really convenient to use a large tool.

I have flood coolant, no TSC.

So you keep the same radial and axial engagement as the climb mill, and reduce the feed to 80% of the climb feed?

Thanks everyone for your input

 

[crossthread82]

I tried that approach, and the part has too many hard to reach spots that it’s not really convenient to use a large tool.

I have flood coolant, no TSC.

So you keep the same radial and axial engagement as the climb mill, and reduce the feed to 80% of the climb feed?

Thanks everyone for your input

Yes 80% feed for the conventional cut, leave everything else the same. Generally when I zigzag it's with a 3/8 or 1/2 endmill about .75-1 deep with around 40% stepover.

 

[apoet]

It’s a VF2SS, so it’s ok rapids.

I don’t understand your second question or statement, are you implying that it’s conservative engagement or too much?

He is saying your radial doc is conservative.

For example, I'm roughing at .1 radial doc with 1/2" tools in 6061 at similar axial doc which sounds/feels like conservative settings to me. I haven't changed the endmill in months.

 

[Chips Everywhere]

He is saying your radial doc is conservative.

For example, I'm roughing at .1 radial doc with 1/2" tools in 6061 at similar axial doc which sounds/feels like conservative settings to me. I haven't changed the endmill in months.

Thanks for the feed back. I was concerned that 1.75" axial a larger radial may be a problem.

 

[DSMWerks]

Good timing on this topic as I am doing a long term 6061 job with a 1/2" end mill for roughing. For the prototype parts I ran climb cut HSM method and chips piled up everywhere in the shop until scrap day. Now it going into production I was planning on trying a corn cob rougher and zig-zag tool path. The part is 16" long and suspended between the 4th axis and a tailstock. It gets a lot of material removed and I worry about chatter. The 3 flute YG1 Alu-Power did well but hoping the corn cob rougher will out perform it.

 

[sinha]

A corn cob rougher allows higher chip loads with reduced chatter. Moreover, it produces smaller chips which can be cleaned up easily. On the negative side, the roughed out surface needs a finishing cut by a regular end mill.

 

[Chips Everywhere]

What kind of tool life are you getting out of end mills running similar parameters as mine? I get about 10-12 hours with my conservative parameters, and the tools break near the holder face on the shank above the flutes. Called Helical about this and they said 10hours is considered good life for my parameters.

 

[DSMWerks]

If asking me I got 35 hrs on YG1 Alu-power 1/2" 3 flute and they were still going but started to be a little noisy. But I was going two passes 1" deep each. I think you are going 1.75" deep? They do make the Alu-power with smooth but a few serrated grooves that may have done better on chips being more compact. Best pricing and free shipping

YG-1 End Mills

YG-1 offers one of the largest selections of Hi-Performance and General Purpose End Mills in the Industry

www.suncoasttools.com