[MetalShavings]

So, if I reduce the depth of my cut, I would then have to do two operations of the same kind? For example; the first at one-half-inch; as apposed to a full inch. And the second at the remaining half-inch of depth to accomplish the full one inch depth of cut? Also: because the depth of cut had been reduced, how does this effect the spindle speed since I would then be cutting shallower than before with my one inch depth of cut?

OR; can the reduced depth of cut be made in lesser increments? For example; I ultimately wanted to go an inch deep. Could I have decreased that one-inch depth of cut to 7/8" or 5/8" deep in order to mitigate that chance of bogging down, and then mill the remainder as a followup operation?

Explaining these things in writing can make them seem more daunting than they really are. As I read your reply, I know that you know what you're talking about but, it's difficult for me to process without seeing it being done.

MetalShavings

[SCzEngrgGroup]

So, if I reduce the depth of my cut, I would then have to do two operations of the same kind? For example; the first at one-half-inch; as apposed to a full inch. And the second at the remaining half-inch of depth to accomplish the full one inch depth of cut? Also: because the depth of cut had been reduced, how does this effect the spindle speed since I would then be cutting shallower than before with my one inch depth of cut?

OR; can the reduced depth of cut be made in lesser increments? For example; I ultimately wanted to go an inch deep. Could I have decreased that one-inch depth of cut to 7/8" or 5/8" deep in order to mitigate that chance of bogging down, and then mill the remainder as a followup operation?

Explaining these things in writing can make them seem more daunting than they really are. As I read your reply, I know that you know what you're talking about but, it's difficult for me to process without seeing it being done.

MetalShavings

Yes, if it's too deep to do in a single pass, I would do it in two equal-depth HSM roughing passes, then a single full-depth finish pass. You will also likely be able to increase the feedrate enough to make up a large part of the extra time the second pass will take. If you're cutting aluminum, you'll almost certainly be spindle-speed limited. I do 90+% of my work with the spindle maxed at 6K RPM.

If you're not using HSMAdvisor, I suggest you get it, and use it. It won't steer you wrong. If you consistently find you cannot to the cuts it recommends, modify the machine model accordingly, and you'll get to a point where it gives you good numbers every time.

Regards,
Ray L.

[wtopace]

So, if I reduce the depth of my cut, I would then have to do two operations of the same kind? For example; the first at one-half-inch; as apposed to a full inch. And the second at the remaining half-inch of depth to accomplish the full one inch depth of cut? Also: because the depth of cut had been reduced, how does this effect the spindle speed since I would then be cutting shallower than before with my one inch depth of cut?

OR; can the reduced depth of cut be made in lesser increments? For example; I ultimately wanted to go an inch deep. Could I have decreased that one-inch depth of cut to 7/8" or 5/8" deep in order to mitigate that chance of bogging down, and then mill the remainder as a followup operation?

Explaining these things in writing can make them seem more daunting than they really are. As I read your reply, I know that you know what you're talking about but, it's difficult for me to process without seeing it being done.

MetalShavings

I agree with Ray. Although your machine should be capable of the 1" deep cut at 0.015" WOC, you should back off and take it in two 1/2" DOC passes and see how it works out.

DOC is a linear multiplier on spindle load, for example: A cut that takes 10% of your HP at 0.5" DOC will take 20% of your spindle HP at 1" DOC and 40% of your spindle HP at 2" DOC (of course this only works in a perfect world, just like how high-school physics are always calculated in a perfect world in a vacuum).

Summary: If your chips are looking good and you're not burning up tools, chances are your RPM and WOC are fine. You can almost always tune your HP usage with your DOC.

[MetalShavings]

I agree with Ray. Although your machine should be capable of the 1" deep cut at 0.015" WOC, you should back off and take it in two 1/2" DOC passes and see how it works out.

DOC is a linear multiplier on spindle load, for example: A cut that takes 10% of your HP at 0.5" DOC will take 20% of your spindle HP at 1" DOC and 40% of your spindle HP at 2" DOC (of course this only works in a perfect world, just like how high-school physics are always calculated in a perfect world in a vacuum).

Summary: If your chips are looking good and you're not burning up tools, chances are your RPM and WOC are fine. You can almost always tune your HP usage with your DOC.

Yea: I had more or less deduced the same thing. What I'm still not clear on -cause I don't own a copy of HSMadvisor and my trial copy has long since expired- is, do the same spindle speeds apply even though I'd be making shallower depths of cut?

MetalShavings

[popspipes]

I didnt see in your posts if you were using coolant? New cutter or sharp one?

Just a guess but i would think maybe cutting dry and the work is heating up and your getting chip weld on the cutter possibly. that would account for the bogging down in later cuts.
6061 tends to get "sticky" when it gets too warm on the lathe if cutting dry, probably similar on the Tormach if cutting dry.

[wtopace]

Yea: I had more or less deduced the same thing. What I'm still not clear on -cause I don't own a copy of HSMadvisor and my trial copy has long since expired- is, do the same spindle speeds apply even though I'd be making shallower depths of cut?

MetalShavings

Yep, spindle speeds relate directly to surface feet per minutes (SFM). Regardless of how deep you're cutting, you still want the cutting edge swinging by the material at the same speed.

There are really 4 main factors in any cut (and lots of little things that influence these):

• RPM - How fast your cutter is flying by the material, this is directly proportional to SFM. RPM/SFM is determined by the tool material (slow for HSS, faster for carbide, fastest for coated carbide) and the work material (slow for stainless, faster for steel, fastest for aluminum)
• WOC - How much material each flute is slicing off as it comes by.
• DOC - How many flutes are engaged at once and how long is your chip? This is your HP multiplier
• IPM - Changing your inches per minute movement speed can increase or decrease the thickness of the chip you're taking. Keep in mind with very small WOC, your cutter is only cutting around 90 degrees perpendicular to your axis of movement (chip thinning), so your chips will have a pre-determined max thickness. Since you know the max chip thickness, you can bump the speed up to that without worrying about burying 90% your cutter (Warning: Doing this isn't the best for a nice finish, but works great for roughing).

Hopefully this demystifies some of the variables. Good luck in the shop!!

Edit: HSM Advisor will give you a great starting point for the above 4 parameters and is well worth the cost. Even with a decent understanding of how the puzzle pieces fit together, I still use HSM Advisor all the time!

[MetalShavings]

I didnt see in your posts if you were using coolant? New cutter or sharp one?

Just a guess but i would think maybe cutting dry and the work is heating up and your getting chip weld on the cutter possibly. that would account for the bogging down in later cuts.
6061 tends to get "sticky" when it gets too warm on the lathe if cutting dry, probably similar on the Tormach if cutting dry.

Generally speaking, what you've stated makes sense. However, I was using coolant and the metal I was machining was 1018 steel. I'm still trying to process the replies I've gotten thus far. Those replies make sense too but, unfortunately for me, I'm the kind of guy that has to see it being done in order for things like this to really make the kind of practical sense I'm looking for.

I may have mentioned this before; I have this sort of dyslexia thing going on whenever I try to learn via the written word. Unless that written word includes alot of pictures to go along with it, it's hard for me to make sense of it; regardless of how well it's written.

Incidentally: Back when I was actually running the part in question using the HSM tool paths I'd generated, I deliberately measured the thickness of several of the Metal Shavings that flew off of my metal stock. Out of curiosity, I wanted to see if they were actually .015" thick. I did it sort of haphazardly; putting my digital calipers on what I thought was the thinest part of the shavings. The thickness of the few shavings I measured averaged close to the .015" that they were supposed to be at. Looking at these metal shavings with the naked eye, you can see that they don't come off the metal stock as a flat shaving. They're more of a pig-tail shaped shaving. I mention this because even though I tried to measure thickness at the flattest points of the shavings, inevitably I'd get measurements thicker than .015".

From these measurements I deduced that perhaps I needed to reduce the WOC.

MetalShavings

[SCzEngrgGroup]

Incidentally: Back when I was actually running the part in question using the HSM tool paths I'd generated, I deliberately measured the thickness of several of the Metal Shavings that flew off of my metal stock. Out of curiosity, I wanted to see if they were actually .015" thick. I did it sort of haphazardly; putting my digital calipers on what I thought was the thinest part of the shavings. The thickness of the few shavings I measured averaged close to the .015" that they were supposed to be at. Looking at these metal shavings with the naked eye, you can see that they don't come off the metal stock as a flat shaving. They're more of a pig-tail shaped shaving. I mention this because even though I tried to measure thickness at the flattest points of the shavings, inevitably I'd get measurements thicker than .015".

Width of cut is only vaguely loosely to chip thickness. Actual chip thickness will almost never be equal to WOC, and can be much greater, or much less, depending on the cut. Chip thickness is a function of many complex factors, but the dominant factors are RPM and feedrate, not WOC.

Proper feeds and speeds calculations, especially for HSM, is a VERY complex subject. That's why you'd be best served, by far, by spending the small amount of money for an HSMAdvisor license. It will pay for itself many times over in shorter machining times, longer tool life, and fewer broken tools. You'll waste a huge amount of time and effort trying to do it yourself.

Regards,
Ray L.

[tmarks11]

....I deliberately measured the thickness of several of the Metal Shavings that flew off of my metal stock. Out of curiosity, I wanted to see if they were actually .015" thick...From these measurements I deduced that perhaps I needed to reduce the WOC

Like Ray said, WOC does not equal Chip Load (sometimes called Chip Load Per Tooth or Feed Per Tooth).

Chip Load = feed rate ( ipm )/( cutting rpm x number of cutting edges) --Note: usually this equation is solved to calculate feed rate based upon RPM and CL.

The tooling manufacturer generally recommends a CL based upon material and cutter diameter. This CL is chosen to maximize insert life, and prevent tool flexing/breaking. For example, in aluminum, a 0.5" endmill generally gets a recommended 0.004" CL, and a 1" endmill gets 0.007".

NOTE: If WOC when edge milling is actually driving CL size, then that means your feed rate is way more than is recommended by the tooling manufacturers.

Here are some good examples
Harvey Tool - Speeds and Feeds Guide | General Machining Guidelines
Niagara Cutter Speed and Feeds

in review:
1. select rpm based upon sfm and tool diameter.
2. select feed rate based upon rpm, CL, material, and diameter.
3. WOC/DOC based upon spindle hp available (this is the calculation where HSM Advisor or G_wizard helps out, the previous two are child's play).

If your chips are too blue or your spindle is bogging down, don't reduce your feed rate. That will make smaller chips, which means your cutter will heat up more and die faster. Instead adjust DOC or WOC so less power is required.

[SCzEngrgGroup]

Like Ray said, WOC does not equal Chip Load (sometimes called Chip Load Per Tooth or Feed Per Tooth).

Chip Load = feed rate ( ipm )/( cutting rpm x number of cutting edges) --Note: usually this equation is solved to calculate feed rate based upon RPM and CL.

And that equation works only for relatively wide cuts, where chip thinning does not come into play. For cuts with a small WOC, the chip will be MUCH thinner than that equation will calculate, which is why you can feed as much as 10X faster when taking a very narrow cut.

Regards,
Ray L.

[MetalShavings]

I'll give it another shot after I've sold off the batch of small parts I made up using conventional milling techniques. With Christmas coming up I'm hoping that alot of air rifles are under the Christmas trees this year. This will assure the sale of my present stock of specialty parts.

The parts in question are closer in shape to the Fish-Shaped parts I posted a zip file on. That's a whole new set of numbers as far as HSM tool paths are concerned. I think someone posted a set of numbers using a three-flute 3/8" coated carbide bit I can try.

I'll let you all know how it works out once I've tried it.

Thanks everyone.

MetalShavings