Spindle speeder worth it?

[Darin]

We run 100,000 of these aluminum 6061 parts. All we do is use a 1/8 endmill with .030 radius to finish this pocket. We have a 10,000 rpm 30 taper machine that we run these on. We currently run about 50,0000 a month and are moving up to 100,000. At $1.00 a piece I am looking into a spindle speeder to get the parts done faster and better tool life. But at $6000 not sure it is worth it. With the 1/8 endmill only taking off about .075 on the walls and .020 on the floors. It is a .300" x .300" at .300" deep pocket that has already been rough out buy another shop before we get it. We run a 10,000 rpm and 10 IPM with a 3 flute carbide endmill now. We get any where from 30 to 1500 parts before endmill breaks. Anyone have experience with these spindles speeders and tool life and run times? Thanks

 

 

http://www.nskamericacorp.com/prod_machineTool_hps.aspx

 

http://www.omgnet.it/mo/index.cfm?lingua=US

[Chris Rizzo]

Hi Darin,

 

30k spindle vs. 10k spindle you'd be breaking tools 3x faster. :lol:

 

I've never used a speeder, but from the math standpoint:

 

-your only running about 300 surface footage with 10k spindle, and your chip load is .0003. Seems weird that your breaking tools at that chip load. How's the run out on the tool? What's the depth cut? Can you ramp contour around that pocket? What is the radius in the corners? If it's '.0625 you might want to consider a 3/32 or 7/64 tool to keep from burrying the 1/8" in the corner.

 

With 30,000 rpm you'd be about 950 sfm, which would help, and theoretically you'd be able to feed at least 3x faster and maintain that .0003 load.

 

Another way to look at it:

 

Even if you save 5 seconds per part, over 100,000 parts that would be over 138 HOURS of run time. At 60$/ hr shop rate that's 8,333 $ right there. Might want to double check my math, seems crazy.

 

Just a few brainstormed ideas there, maybe someone else can chime in too. hth

[Joe788]

Holy moly, 100,000 of that part per month? Hope you're loading it with a robot!

 

As Colin mentioned, .0003 chipload seems a little low. What does your toolpath look like?

[Guyinthedesert]

What kind of endmills are you using?

[Guest CNC Apps Guy 1]

Buy the speeder. They are worth it.

[Darin]

Hi Darin,

 

30k spindle vs. 10k spindle you'd be breaking tools 3x faster. :lol:

 

I've never used a speeder, but from the math standpoint:

 

-your only running about 300 surface footage with 10k spindle, and your chip load is .0003. Seems weird that your breaking tools at that chip load. How's the run out on the tool? What's the depth cut? Can you ramp contour around that pocket? What is the radius in the corners? If it's '.0625 you might want to consider a 3/32 or 7/64 tool to keep from burrying the 1/8" in the corner.

 

With 30,000 rpm you'd be about 950 sfm, which would help, and theoretically you'd be able to feed at least 3x faster and maintain that .0003 load.

 

Another way to look at it:

 

Even if you save 5 seconds per part, over 100,000 parts that would be over 138 HOURS of run time. At 60$/ hr shop rate that's 8,333 $ right there. Might want to double check my math, seems crazy.

 

Just a few brainstormed ideas there, maybe someone else can chime in too. hth

 

 

Thanks for the info Chris. They are running a 4 flute garr endmill now. The three flute broke to fast. I haven't ran my program to try my path yet. I am waiting for the super high accurate holder I ordered to get here first. I think the code was done with BobCad a while back. The pocket is about .300 deep and it only takes about .075 off the walls and .020 to .030 on the floor. I attached a picture of the rough and finished part.. The path they use had .062 radius corners. The print will allow up to a .074 radius. So I programmed for that. That might help the life. My path starts in the center full depth and takes multi passes (I think 3 passes) till I get to the .300 width. Would I be better to ramp down? The fixture holds 32 parts they make about 2000 a day. But I need to get close to 4000 to make the 100,000 a month. I am designing a different way to hold them in Solidwaorks right now using chick air vices. It will do 12 at a time and be on a pallet changer Kia machine. Or maybe a Mazak 410c with pallet changer. They have a full time employee that just runs this part. I wish I could try out the spindle speeder to see if it will beat my new program and high precision holder at 10,000 rpm 25 to 35 ipm. That is what I will try.

[Darin]

What kind of endmills are you using?

We are using Garr tool 4 flute .030 radius (The 3 flutes broke fast) but I have high end Ultra endmills and Prototyp endmills coming to try.

[Guyinthedesert]

We are using Garr tool 4 flute .030 radius (The 3 flutes broke fast) but I have high end Ultra endmills and Prototyp endmills coming to try.

 

 

Try a high helix, like a 48 deg dataflute.

[35K chipper]

Darin,

this is what i use every day. harvey tools .125 3flt variable helix carbide diamond coat with .005 rad. and .375 loc SFM 1154.29

35000 rpm at 70.35 ipm .0007 cl/flt .0125 step over. this is my roughing tool. tool life i dont know its been running for 3 months.

in 6061 T6. i use the 10% radial rule. get that NSK air speeder!!! there are times when i wish i had more than 35k rpm's.

.

.

35k

[K2csq7]

For our big machines (all we have) we only get about 2k RPM out of the spindle, then the W axis starts to grow and within 20 min. the Z offset can be off by up to .015".

We have a BIG dishowa (sp.) 5.67:1, I use that regularly. We also have a 60K RPM air spindle we use for wicked small stuff.

With quantities like 100k/ month I would be looking to save every tenth of a second I could....

[jeff]

4 flute? ewwwwwww.

Try a 2 or 3 flute OSG Blizzard, uncoated.

I have no experience with speeders, but 10k CAN do the job, you want at least 15k to be efficient for that size of an endmill.

 

Are you using coolant? air blast?

 

Oh and get a stubby, they are stronger.

[McLaren]

Can I get some more info? How many hours per day does it run? At 8 hours for 2000 parts that would be 15 seconds per part. Taking 1 rough pass and 1 .03" finish pass at 10 ipm would be like 7 seconds per part. 3 passes would be like 10 seconds per part. Running 32 parts at a time and losing 5 seconds per part is 160 missing seconds. Where are those 2.5 minutes? What is the total cycle time per set? Per part? On a pallet changer now? If so what is pallet change time? If not how much time to switch fixtures? How much lost production to switch broken tools?

 

Like Rizzo said, if you don't fix anything else you will just break endmills 3x faster. I think there are some other places to improve the process first. It looks like you have 2.5 hours of missing time each day that at least a part of could be gotten back.

[McLaren]

The reason I am asking these questions is because with 3 passes you are dealing with like 1.5 inches of cut length. With accel/decel ramps it's just not that much travel and I doubt you can double your feedrate and cut your cycle time in half. As a test try this with no parts in the fixture:

Run through a cycle at 100% and get a exact machine time.

Double the feedrates everywhere and run it again.

Post back your results.

[Newbeeee™]

Darin,

this is what i use every day. harvey tools .125 3flt variable helix carbide diamond coat with .005 rad. and .375 loc SFM 1154.29

35000 rpm at 70.35 ipm .0007 cl/flt .0125 step over. this is my roughing tool. tool life i dont know its been running for 3 months.

in 6061 T6. i use the 10% radial rule. get that NSK air speeder!!! there are times when i wish i had more than 35k rpm's.

.

.

35k

 

Chip,

If it's lasted 3 months, you're not pushing hard enough. I mean c'mon, it's a solid 'ol 1/8th cutter and you're only running it at 70 inch feed

 

Oh, and don't be greedy. I'm sure 35K revs are more than enough

[Darin]

4 flute? ewwwwwww.

Try a 2 or 3 flute OSG Blizzard, uncoated.

I have no experience with speeders, but 10k CAN do the job, you want at least 15k to be efficient for that size of an endmill.

 

Are you using coolant? air blast?

 

Oh and get a stubby, they are stronger.

 

 

The depth of the pocket is about .300. A stubby 1/8 is under a .250 loc. So I need a .375 loc of cut to machine a full depth. We are using coolant. Not through spindle.

[Chris Rizzo]

More brainstorming- I'd concentrate on the total cut time, and not so much the linear inches traveled.

 

A light ramp (.04) at a really fast feedrate may provide a low-tool load situation.

Or maybe a dynamic contour at full depth to nibble out the corners within .002, then a 150 ipm finish pass.

How about maybe plunging straight into the corners, then a quick contour? 3 Totally different methods there, but worth some experimenting.

My philosophy in machining (and life in general) is no matter how good a process can seem , there ALWAYS will be a better way to do something. I've spent days trying to save seconds off parts (and driven myself nuts in the process).

 

 

35k chippers' numbers seem great too, you could prolly roll with those.

 

more2 cents

[Darin]

The reason I am asking these questions is because with 3 passes you are dealing with like 1.5 inches of cut length. With accel/decel ramps it's just not that much travel and I doubt you can double your feedrate and cut your cycle time in half. As a test try this with no parts in the fixture:

Run through a cycle at 100% and get a exact machine time.

Double the feedrates everywhere and run it again.

Post back your results.

 

 

I haven't yet run my new program which only has one pass. The old program goes through all 32 parts rough and then goes back and finishes all of them. It runs on a vacuum fixture that he loads will it is running. So the lost time is the two passes I think. My program will just have one pass at full depth with 3 or 4 .015 multi passes and be done. The times he gave me aren't adding up right...I will have to watch it closer or run it my self to see exact times.

[Darin]

More brainstorming- I'd concentrate on the total cut time, and not so much the linear inches traveled. A light ramp (.04) at a really fast feedrate may provide a low-tool load situation. Or maybe a dynamic contour at full depth to nibble out the corners within .002, then a 150 ipm finish pass. Totally different methods there, but worth some experimenting.

 

35k chippers' numbers seem great too.

 

more2 cents

 

 

Good idea Chris. I will try both ramping and full depth cut multi passes to see the time difference. I have definitely decided to get a spindle speeder. We got another job running 100's of .025 drill holes... I can use it on also.

[Chris Rizzo]

I just edited my post up there and added some more ideas.

[McLaren]

Plunge milling the corners is always a good one. Just don't forget that with that size corner radius there is going to have to be 2 passes on the floor no matter what to get rid of cusp.

 

And again, I would see what your machine can actually feed at in that small of a space. See if you can run it empty at 20ipm and get your cut time reduced in half, then try 40, 80 160. Your are going to hit an accel/decel limit quicker than you think. Those are only .150" long lines best case.

[K2csq7]

Don't use multi-passes, use dynamic... 50million times better for tool life/surface finish... Well at least 100 times better

[Roger Peterson]

without seeing exactly how your cutting it, it seems really odd that you are breaking tools. Especially at unpredictable intervals. The only place you could be breaking the tool is going into one of the corners. Dynamic contour is a great place to start and let it peel the corner out of there. There are a lot of really good endmills for this from a lot of different companies, polished and coated, like Harvey, ISCAR, Benchmark, etc... Don't be afraid to have a tooling vendor or two come in and try some of their tools.

 

While a speeder would certainly speed things up, you aren't running a sub 1mm cutter. You have 10K for a .125" endmill which should be plenty to eliminate the breakage and speed things up by switching to the dynamic contour.

 

 

Get a balanced holder, it can be a collet holder, they help a lot with small and smallish cutters.