High Speed Machining

[EricJ3D]

Not sure you could really call this high speed but I figured I would ask the question. I've been asked to quote a larger than usual job of 100 pcs in 6061. Normally I would pass but the geometry seems pretty simple and I could run these in batches.

Attached is a picture of the batch, it will fit nicely on a 8in X 16in plate. The parts are 1in tall and spaced evenly at .625" between parts. The customer is flexible with part modifications required for tooling fixtures. I work with SprutCAM 11 I've been looking into torchoidal tool path such as this video:





This would be for material removal in between the parts. In the past I have tried out plunge roughing as per Steve Seebold's parameters with great results but I'm concerned this might be a little rough on the endmil and the machine. Working with G-Wizard I get the following parameters for a material removal rate of about 2.5 cubic inches.

The results were less than spectacular. Lots of chatter, lousy sunfish finish and I wasn't running any where near 90 IPM. I'm running a souped up flood coolant so chip evacuation is not a problem. I am going to try out a YG-1 3 flute endmill I just ordered. https://www.amazon.com/gp/product/B0...?ie=UTF8&psc=1

So my question is should I forget about torchoidal tool paths and go with a more traditional method of slotting? Is plunge roughing a little bit too much for this project?

Any info is greatly appreciated


Thanks

Eric

Similar Threads:

• High Speed Machining
• Newbie- high speed machining (High RPM)
• High Speed Machining??
• Need Help!- High speed machining
• Welcome to high speed machining

[SCzEngrgGroup]

Back off on depth, and I suspect you'll be able to actually increase feed. At 0.025" WOC, I can easily do 1/2" DOC at 150 IPM. At 0.05" WOC, I do 1/2" DOC at 110 IPM. That's using a cheap ($12) HSS 2-flute, and neither is stressing the machine or the tool in the slightest. Use a helical entry with 5 degree ramp to do most of the initial removal in the pocket, using as large a radius as will fit, while completely clearing the center of the pocket. Unfortunately, your MRR is going to be limited by your machines limited RPM and feedrate, not by the tool.

Something else to try - with HSM, you can often get away with using a 4-flute tool, even for pocketing, which allows you to increase feedrate even further. So, you might get a better result using a 4-flute tool, and greater depth.

FWIW - I've always found HSMAdvisor to be much better at coming up with optimal feeds and speeds than GWizard.

Regards,
Ray L.

[IMT]

With the parts spaced at .625 you'll be roughing a .605 wide slot if you leave .010 for finishing. Using HSM tool paths with a .500 EM the radius is very small and thus the actual angle of engagement is much greater than if you were cutting straight with the same step over value. In this case the tool path radius is .053 (.605-.500)/2, with a step over of .025 the angle of engagement is 63 degrees where as in a straight cut the angle is only 26 degrees. Using that small a radius more than doubles the effective step over (actually it increases it .138 in this case! >5X). No surprise it chattered.

FWIW, I rarely use HSM for slotting or pocketing in aluminum. Much faster to full slot using small DOC and a inexpensive roughing EM.
I would use a stub length 3 or 4fl roughing EM (~$10) and full slot (3800rpm, .100 DOC, ~60IPM), with lots of flood coolant.

[Steve Seebold]

I would create a hole pattern with about a 40% step over on the diameter of the cutter and plunge ruff leaving.015 to .020 for finish machining.

I ruff like that all the time and it's way faster than side cutting.

[mountaindew]

I would create a hole pattern with about a 40% step over on the diameter of the cutter and plunge ruff leaving.015 to .020 for finish machining.

I ruff like that all the time and it's way faster than side cutting.

I started using this method after Steve mentioned it a few years ago. Works great for big or small pockets in hard or soft materials and drilling you can get real aggressive because your machining straight down and drill bits are cheaper then end mills for hogging out pockets.

[zero_divide]

I agree with those suggesting NOT using the low engagement HSM stye toolpaths for anything close to slotting.

IMO just leave 0.55" between parts and then using a 3 flute carbide(or even HSS) endmill slot it and then finish sides.

The reason you got crap finish is that a 2 flute HSS cutter is just too damn flimsy. If you add the flimsiness of the machine itself, it is no wonder you got not so good results.

So when slotting with a 3 flute you can go around 5000 RPM and about 30 ipm as deep as your Horse Power allows. With Coolant.

If you have a higher helix endmill you will not have to worry about chatter either.

I am not so sure plunge milling would be any good because you would be wasting a lot of time on accelerations and useless retract. Plus the wear on the z axis and.

[wildwhl]

Obviously I don't know the dimensions, whether you require chamfers, tolerances etc. but I'd have to honestly consider going after these simply in rows of 6 or 7 from bar stock spread across a pair of vises (assuming you have such). Simple tool paths, nothing fancy, and then flip them over and face mill the balance of the material. Just a thought.

I'd be curious to hear time estimates on these, too? I come up (just really quick conservative tool paths) with about 25 minutes each group of 6 (surely can be quicker) assuming chamfers on all edges. I'd slip in the *bottom* chamfers from the top if possible, but if the chamfers aren't necessary probably closer to ~20 minutes (per 6) this way...Just from the hip, using 3 fl .500 and .250 endmilss, spot drill, and .125" twist drill as example. This would be on an 1100...and generally I find I cut 35-40% time off the initial tool path after cutting the first batch.

Depending on what the inside radius is, I might even program the whole thing using a .250 3 flute end mill and whatever drills are required. Let the ATC have the fun while I do some other *work*.

WW

[EricJ3D]

Thanks Guys for all the great suggestions and the time you have put into this thread. Normally I would run this at a (very) conservative rate since time normally doesn't matter, but at 100 pcs I know I have to pick up the pace. I'm running an 1100 and I plan on making some practice runs a little later in the week.

Ray
I've never run those kinds of feeds and speeds (or remotely close). I'm going to make a few samples on a 1" part and see how the machine responds. I'm pretty excited with the new flood coolant upgrades I finished this weekend. I'm slightly intimidated by those numbers since I'm new to this and just last month I had my first real crash at fairly high speeds. Minimal damage....thank you E-Stop.

I also recently purchased HSMAdvisor due to it's great reviews, but have not had a chance to work with it much.

IMT
Thanks so much for crunching those numbers, I see exactly what you are saying. I have a ton of 1/2" stub end mills which look and feel like new that I purchased from our retiring prototype machinist at work. I will try a few out with your numbers.

Steve
Thanks a lot for this information. I have tried your parameters out previously with great results on smaller end mills 1/4" or less. I started breaking them around 1/8" dia or less so I tried pecking and that seemed to get me out of a jam. 1/4" EM just hauled!

So for this I would start off with 1/2" drill then step over 40% with a 1/2" EM leaving .015 to .020 for clean up. Do you have any recommendations for plunge feed rate? The 1100 started to groan a bit on with the 1/4" EM but I don't remember what I was plunging at.

Mountain Dew
First off let me say thank you for all the tireless posts you have made on SprutCAM. I'm a CAD guy and I seriously would not be where I am now with this friggin' software without all your posts. Jacob is great but your posts and screen shots are top notch.

One question, are you drilling out most pockets? I've used Steve's parameters but he only calls out drilling as the first operation then following up with the same diameter EM at a 40% step over. I would be interested in trying completely drilling then following up with an EM.

Zero Divide
Thanks for your input on this. I have a 3 flute on the way from YG-1, looking forward to trying it out. I guess the consensus is not to use HSM tool paths for this particular configuration. I am going to try out your numbers. I purchased HSM Adviser but have not worked with it much. Hope you don't mind if I bug you a little when I have a little more time to start working with it.

Wildwhl
Thanks a lot for your suggestions and I had to laugh. At work, I just showed the machine shop manager what my plan was and he basically told me he would fire me for wasting so much precious metal. He did recommend running some more simple tool paths with bar stock and without HSM. Lots of flood coolant for chip evacuation. Getting a second vise would be no problem but I will try to run a few samples on the single vise I have now. Thanks a lot for running this though your CAM program, I now have a few time numbers to shoot for.



Guys, thanks so much for your time and input on this. You're really helping a rookie out.

Eric

[AUSTINMACHINING]

I think I would space them .4" apart and use a .375 end mill with a slotting toolpath. Predrilled the inside and hsm out to the edge. Don't know the inside radius, but if it's close to the endmill radius, drill/relive the corners to avoid chatter on the finish pass.

BTW,
I just got a 1/2" ZRN coated serrated rougher from Maritool. Spindle load dropped 25% on the same cut as the YG1. But YG1 work great every where, and leave a stellar finish. Still the best bang for the buck IMO.