[Babba]

Hope you've not all got sore heads (hic)!

I'm machining a profile from 25mm deep 6082 Ally and despite lots of experimenting I'm still left with a finish that has to be sanded out.

I'm using a 10mm Carbide TiAN coated 2 flute end mill running at 3000rpm, 3mm depth, 130mm per minute on a Syil SX3. I don't have flood coolant but have tried cutting with paraffin (brushed on), compressed air & even dry.

What's causing this finish?

[orizaba]

Hope you've not all got sore heads (hic)!

I'm machining a profile from 25mm deep 6082 Ally and despite lots of experimenting I'm still left with a finish that has to be sanded out.

I'm using a 10mm Carbide TiAN coated 2 flute end mill running at 3000rpm, 3mm depth, 130mm per minute on a Syil SX3. I don't have flood coolant but have tried cutting with paraffin (brushed on), compressed air & even dry.

What's causing this finish?

I should start by saying I'm not a real machinist, I just play one on TV.
Having said that, It looks to me like the end mill flexing. I was having the same problem on one of my projects.
How much material are you removing on your last pass?
I ended up using a .750 solid carbide 3 flute endmill, removing .005'
cutting .400 deep on the final pass in a conventional pattern (not climb milling) at 1500 rpm's moving 20 ipm.
I was cutting 7075 and it gave me a very nice finish
I hope this isnt bad advice.

Matt

[WayneHill]

Matt,

It is good advice. Finish stock pass is a good recommendation.

[Geof]

It is probably a combination of the tool and machine flexing probably combined with some minuscule vibrations from the spindle bearings.

Take a finish pass using a four flute cutter removing only something like 0.02mm. If you have spare material to play with you could try changing the spindle speed to see if it makes a difference.

[fretsman]

Just out of curiosity, do you have a picture of an aluminum finish that you're trying to achieve?

Dave

[ataxy]

yes that is probably due to vibration in the setup somewhere make sure the gibs are well tighten. as other have asked what is the width of cut you used.

mostly make sure the z gib is tight by lowering the spindle on a aluminum block on the table to put a bit of upward pressure on the head and tighten the gib on my x4 i was able to turn the screw of the z gib by a turn and a half this will reduce most if not all the chatter you might get from the head assembly, is this a first time occurrence or as it alway bee doing this.

[dertsap]

I'm using a 10mm Carbide TiAN coated What's causing this finish?

you'd be better off using an uncoated endmill

[scudzuki]

Climb milling is preferrable for a finish pass on a profile unless your machine has excessive backlash.
Joe

[mc-motorsports]

That's normal for a benchtop machine. Spindle flex, vibration, you're really not going to get around it. You can take 2 or 3 passes, like 12mm deep then 13mm deep, but then you'll probably end up with a little step on the part. It's just machine flex and vibration.

Don't use coated enmills on aluminum, and HSS will give better finishes but wear out faster.

A Mori Seiki machine costs a hell of a lot more, but it's night and day when your trying to ship parts with a as machined finish, not to mention tolerancing, feedrates, reduced vibration... What I'm saying is you just have to work with what you have. All things concidered, the finish looks fine. It's understandable that you would want to polish it, but for off the machine on anything less than heavy iron, I would say you did ok.

[CarbideBob]

Get an endmill made to cut aluminum.

Who the heck sold you a TiAN coated endmill for cutting aluminum?
The aluminum in the coating will cause the workpiece material to bond to the endmill. Dertsap is right, you'll do better with an uncoated tool. The only coatings you should consider for aluminum are ZrN or TiB.

A endmill designed for aluminum has higher rake and clearance angles than a steel cutting tool to provide a cleaner shearing action, lower tool pressures, and less rubbing from the increased "springback" that you get when cutting aluminum. Aluminum cutting tools will also have polished flutes to reduce friction and chip welding. Micrograin C-3 (low cobalt) carbides will give the best life.

Climb mill if possible. Try using WD-40 for a lubricant.
Bob

[ataxy]

That's normal for a benchtop machine. Spindle flex, vibration, you're really not going to get around it. You can take 2 or 3 passes, like 12mm deep then 13mm deep, but then you'll probably end up with a little step on the part. It's just machine flex and vibration.

Don't use coated enmills on aluminum, and HSS will give better finishes but wear out faster.

A Mori Seiki machine costs a hell of a lot more, but it's night and day when your trying to ship parts with a as machined finish, not to mention tolerancing, feedrates, reduced vibration... What I'm saying is you just have to work with what you have. All things concidered, the finish looks fine. It's understandable that you would want to polish it, but for off the machine on anything less than heavy iron, I would say you did ok.

true you can expect the same finish as a industrial size machine but he should still be able to get better finish then this

[LongRat]

25mm is deep. You need to maximise tool stiffness to cut that deep when doing your (essential) finishing pass at full depth. I would suggest the finish pass to remove a skin thickness of 0.1mm at 130mm/min with the spindle speed maxed out. Use a carbide tool (much stiffer) of the largest diameter possible. Climb milling is essential to get a better finish than you already have. Also, if possible mount the material as close to the table surface as possible, so you are cutting with the head right at the bottom of the z column. This will dramatically increase the stiffness of your set-up. You WILL be able to improve on what you have, I've got better finishes than that out of my X2 cutting similarly deep and the X3 is a lot more rigid.

[BobWarfield]

What a fascinating thread. I always wish for more pictures and a more methodical approach on surface finish issues. Some day I may try to do that.

Cheers,

BW

[LongRat]

Unfortunately I don't have any pictures to hand of anything as deep as 25mm. Here are some parts assembled up which I did, the maximum thickness is about half of that. Most of these parts were machined with a 6mm 2 flute solid carbide end mill, finishing pass at full depth, offset 0.2mm, feed 100mm/min. For these parts I didn't have my machine converted to belt drive, so spindle speed would have been around 2000 RPM.



Some of these edges are extruded section and not machined, but you get the idea.