[spork]

Let me apologize in advance if this is a stupid question or already covered 100 times. I've done some work on a ShopBot, but will be doing my first project on a Tormach Mill shortly. I need to machine a part out of 6061-T6 that will be roughly speaking a 1" thick, 3" diameter disk.

I assume I'll clamp a 4" x 4" chunk of aluminum in the vice, and cut out my part, leaving tabs to hold it in the larger chunk.

I don't know where to start to figure out the spindle or feed speed (or cut depth per pass). I've got to believe this is one of the most common materials to machine. I'd appreciate it if someone could give me a set of starting numbers or point me in the right direction.

Thanks.

[TXFred]

Need more info.

What tool are you using to cut the part? To correctly calculate feeds and speeds, we would need to know the following.

Tool diameter.
Number of flutes
Length of the flutes.
Material the tool is made of.
What coating the tool has, if any.
Will you be running flood coolant?
Based on the description of how you're going to make the parts, I'm assuming a full width cut (A.K.A. slotting). Is that correct?

Given that info, we can give you some numbers to try.

I suggest you look into GWizard, which can calculate these things for you. That's what I'm going to use to give you some numbers once I get your reply.

Frederic

[Steve Seebold]

Is it possible for you to post a sketch of what you're trying to accomplish here, along with the information requested by TXFred in his reply.

[SCzEngrgGroup]

RPM should be calculated based on the tool material, tool diameter, and the work material:

RPM = SFPM * 12 / ( PI * ToolDiameter )

This can be simplified to:

RPM = SFPM * 4 / ToolDiameter

Typical SFPM Values for HSS Tools:
Cast Iron 30-50
Mild Steel 80-100
Aluminum 400

For Carbide tools, triple the HSS values

So, for a 1/2" HSS endmill in aluminum RPM = 400 * 4 / 0.5 = 3200 RPM

Feedrate = RPM * #Teeth * Chipload

Chipload can be approximated by 0.008 * ToolDiameter, until you get into small, fragile tools (under 1/8"), where the chipload needs to be reduced further.

So, for a 1/2" 2-flute HSS endmill, Chipload = 0.008 * 0.5 = 0.004"

Feedrate = 3200 * 2 * 0.004 = 25.6 IPM

If you work through the calculations, you'll see that until you get into very small, fragile tools, a large diameter tool and a small diameter tool will use the same feedrate, with only the RPM changing. So, if a 1/2" endmill uses 3200 RPM at 25.6 IPM, a 1/4" endmill will use 6400 RPM at 25.6 IPM. If you can't reach that RPM then use the highest RPM you can, and reduce feedrate proportionally. So, if you can only go 4000 RPM, then the feedrate becomes 25.6 * 4000 / 6400 = 16 IPM.

As a rule of thumb, when slotting, if your DOC exceeds 1/2 the tool diameter, you need to start reducing feedrate. As a rule of thumb, reduce feedrate by half at DOC = one diameter. So, for the above endmill:

DOC = 0.25" ==> Feedrate = 25.6 IPM
DOC = 0.50" ==> Feedrate = 12.8 IPM

When making very light cuts (< 1/4 tool diameter), feedrate needs to be increased, to compensate for chip thinning. For the above endmill, if the width of cut is 0.01", you should at least double the feedrate.

Follow the above, and you'll get reasonable starting RPM and feedrate. Getting optimal values requires experimentation, as the best values are different for different machines, and different situations, and can only be learned through experience.

Contrary to common belief, and many peoples intuition, increasing RPM, or reducing feedrate is NOT "easier" on the tool or the machine. Both will reduce chipload, and low chipload leads to the tool heating up. The best way to keep the tool cool is to keep the chipload as high as possible, and the heat will be carried away by the chips, leaving the tool cool. The most common result of a too-low feedrate or too-high RPM is chips welding to the tool. The natural reaction to this is to reduce feedrate, which is exactly the wrong thing to do. When RPM and feedrate are correct, the tool will only get hot on very aggressive cuts - the kind these benchtop machines are not really capable of.

Also, on these benchtop machine with limited RPM, you'll save a lot of money by using HSS tooling, rather than carbide. HSS is more rugged - carbide chips VERY easily. The only time carbide might be appropriate is on small diameter tools (under 1/4"), where the extra stiffness can be helpful. But, on average, GOOD HSS tools will cost less than cheap carbide tools, they'll last longer, and will cut every bit as well. On a stiffer machine, with higher RPMs, carbide can be very beneficial.

My normal roughing cut in 6061 is a 1/2" HSS 2-flute endmill, 3300 RPM, 30 IPM, 0.20" DOC, 0.500" WOC. For finishing, I use 5000 RPM, 50 IPM, any depth, 0.010" WOC. If you can't go that fast or deep, reduce RPM, scale the feedrates by your chosen RPMs, and you should be OK.

Regards,
Ray L.

[spork]

Hey guys - thanks a ton for all the good info. This will give me a great starting point.

What tool are you using to cut the part?

Not sure to tell you the truth. I think we have some reasonable end-mills at the office, so I'll try and pick one based on the info you guys have provided. I think they may also have bits at the TechShop, but I'm not sure. I'll report back.

To correctly calculate feeds and speeds, we would need to know the following...

Most of that I don't know until I select a bit. I will be running coolant.

Based on the description of how you're going to make the parts, I'm assuming a full width cut (A.K.A. slotting). Is that correct?

The top surface will be milled down maybe .250" leaving some cylindrical dogs. The rest will be full width cuts.

I suggest you look into GWizard, which can calculate these things for you. That's what I'm going to use to give you some numbers once I get your reply.

I'll look for that. Thanks.

Is it possible for you to post a sketch of what you're trying to accomplish here, along with the information requested by TXFred in his reply.

I'll take a crack at it, but it will be very unconventional. I don't tend to use CAD/CAM software. Instead I write my own code to produce the cut file directly. But maybe I can make a sketch by hand and post a pic.

If you work through the calculations, you'll see that until you get into very small, fragile tools, a large diameter tool and a small diameter tool will use the same feedrate, with only the RPM changing.

Thanks. That's a very useful tip. Perhaps I'll use the largest diameter bit that will fit between the dogs. I have to take my clutch apart and take some measurements to see what that is, but I will do that. If the distance between the dogs is too small, I'll just leave out every other dog.

As a rule of thumb, when slotting, if your DOC exceeds 1/2 the tool diameter, you need to start reducing feedrate.

Perfect. That's exactly the sort of thing I need to know. Thanks.

When making very light cuts (< 1/4 tool diameter), feedrate needs to be increased, to compensate for chip thinning. For the above endmill, if the width of cut is 0.01", you should at least double the feedrate.

When you talk about light cuts, do you mean shallow cuts, small step-over, or both?

Contrary to common belief, and many peoples intuition, increasing RPM, or reducing feedrate is NOT "easier" on the tool or the machine.

Understood. I'm FAR from an expert on this, but I've learned that lesson on the ShopBot CNC router and on the DRO mill we have at the office. That's one of the reasons I really want to have some good starting points to work with. Otherwise I might be tempted to just start very slow and increase feed rate as I gained experience. Of course that's a lousy approach.

When RPM and feedrate are correct, the tool will only get hot on very aggressive cuts - the kind these benchtop machines are not really capable of.

I'm not sure if this Tormach is a "benchtop" machine. It's a pretty big boy.

My normal roughing cut in 6061 is a 1/2" HSS 2-flute endmill, 3300 RPM, 30 IPM, 0.20" DOC, 0.500" WOC. For finishing, I use 5000 RPM, 50 IPM, any depth, 0.010" WOC. If you can't go that fast or deep, reduce RPM, scale the feedrates by your chosen RPMs, and you should be OK.

Thanks a million! That right there should get me started. I'll check on my bit options.

[Steve Seebold]

RPM should be calculated based on the tool material, tool diameter, and the work material:

RPM = SFPM * 12 / ( PI * ToolDiameter )

This can be simplified to:

RPM = SFPM * 4 / ToolDiameter

Typical SFPM Values for HSS Tools:
Cast Iron 30-50
Mild Steel 80-100
Aluminum 400

For Carbide tools, triple the HSS values

So, for a 1/2" HSS endmill in aluminum RPM = 400 * 4 / 0.5 = 3200 RPM

Feedrate = RPM * #Teeth * Chipload

Chipload can be approximated by 0.008 * ToolDiameter, until you get into small, fragile tools (under 1/8"), where the chipload needs to be reduced further.

So, for a 1/2" 2-flute HSS endmill, Chipload = 0.008 * 0.5 = 0.004"

Feedrate = 3200 * 2 * 0.004 = 25.6 IPM

If you work through the calculations, you'll see that until you get into very small, fragile tools, a large diameter tool and a small diameter tool will use the same feedrate, with only the RPM changing. So, if a 1/2" endmill uses 3200 RPM at 25.6 IPM, a 1/4" endmill will use 6400 RPM at 25.6 IPM. If you can't reach that RPM then use the highest RPM you can, and reduce feedrate proportionally. So, if you can only go 4000 RPM, then the feedrate becomes 25.6 * 4000 / 6400 = 16 IPM.

As a rule of thumb, when slotting, if your DOC exceeds 1/2 the tool diameter, you need to start reducing feedrate. As a rule of thumb, reduce feedrate by half at DOC = one diameter. So, for the above endmill:

DOC = 0.25" ==> Feedrate = 25.6 IPM
DOC = 0.50" ==> Feedrate = 12.8 IPM

When making very light cuts (< 1/4 tool diameter), feedrate needs to be increased, to compensate for chip thinning. For the above endmill, if the width of cut is 0.01", you should at least double the feedrate.

Follow the above, and you'll get reasonable starting RPM and feedrate. Getting optimal values requires experimentation, as the best values are different for different machines, and different situations, and can only be learned through experience.

Contrary to common belief, and many peoples intuition, increasing RPM, or reducing feedrate is NOT "easier" on the tool or the machine. Both will reduce chipload, and low chipload leads to the tool heating up. The best way to keep the tool cool is to keep the chipload as high as possible, and the heat will be carried away by the chips, leaving the tool cool. The most common result of a too-low feedrate or too-high RPM is chips welding to the tool. The natural reaction to this is to reduce feedrate, which is exactly the wrong thing to do. When RPM and feedrate are correct, the tool will only get hot on very aggressive cuts - the kind these benchtop machines are not really capable of.

Also, on these benchtop machine with limited RPM, you'll save a lot of money by using HSS tooling, rather than carbide. HSS is more rugged - carbide chips VERY easily. The only time carbide might be appropriate is on small diameter tools (under 1/4"), where the extra stiffness can be helpful. But, on average, GOOD HSS tools will cost less than cheap carbide tools, they'll last longer, and will cut every bit as well. On a stiffer machine, with higher RPMs, carbide can be very beneficial.

My normal roughing cut in 6061 is a 1/2" HSS 2-flute endmill, 3300 RPM, 30 IPM, 0.20" DOC, 0.500" WOC. For finishing, I use 5000 RPM, 50 IPM, any depth, 0.010" WOC. If you can't go that fast or deep, reduce RPM, scale the feedrates by your chosen RPMs, and you should be OK.

Regards,
Ray L.

I don't understand where these 3300 RPM, 30 IPM .200 DOC are coming from. These are cuts that would require a 20 horsepower machine, and that certainly ain't no Tormach.

Don't get me wrong. I love my Tormach and I just run the hell out of it, but not at those feeds and speeds. I run my Tormach 40 to 70 hours per week.

I haven't the last couple of weeks. I got bit by that frigging bug that's been going around.

A lot of times my wife will come out in the garage and ask me "how late you gonna work tonight" and my answer is always "I dunno, what's on TV".

When I try the feeds and speeds mentioned above, my cutter will pull down out of the collet and scrap the part. I have found that if I use a 1/2 inch 3 flute YG end mill, I can run along at 4500 RPM, .05 DOC, .375 width. Yes, it takes a little longer to make my part that way, but I'm not doing this to make a lot of money. If I were, I would have bought a Mazak instead of my Tormach.

Drilling holes, now that's a different story. All your pressure is straight down, so as long as you don't stall the machine or break the drill, then just let her rip.

If I have a lot of material to remove in a slot or pocket, I will make a drilling routine and plunge ruff most of the material out only leaving about .025 stock on the sides and bottom, then I'll take a semi finish cut leaving .005 on the sides and bottom, then I will slow down to about 3,000 RPM and reduce the feed rate to about 15 IPM for the final finish.

I have learned a lot of this stuff since I got my Tormach by trial and error.

OK, it's now 2:00 AM

Night all.

[Steve Seebold]

I'll take a crack at it, but it will be very unconventional. I don't tend to use CAD/CAM software. Instead I write my own code to produce the cut file directly. But maybe I can make a sketch by hand and post a pic.

Can you draw a sketch on a piece of paper, scan it and post it here?

If you can, great. Let us give you a helping hand. I can't speak for the others, but I love to help out, up to and including showing you how to do some programming, or even making a couple of programs for you.

Where do you live? I live in San Clemente, CA.

If you send me a PM, I'll send you my phone number and we can talk about what you're trying to accomplish.

My business consists of making parts for1/5 scale remote control gasoline powered race boats, cars, trucks and buggies.

When I bought my machine I had visions of making enough money to replace the money I took out of savings to buy the machine. Then I woke up one morning and smelled the coffee realizing along the way "hey, this is supposed to be a hobby" who cares if you replace that money, so I finished the work I had in the shop and decided to now be really picky about the outside work I take in from now on.

I used to take whatever kind of work that came along, and believe me, I got some real crap.

NO MORE.

Steve

[SCzEngrgGroup]

I don't understand where these 3300 RPM, 30 IPM .200 DOC are coming from. These are cuts that would require a 20 horsepower machine, and that certainly ain't no Tormach.

Steve,

Sorry, but your calculation is way off the mark. What I specified is barely a 1HP cut. I can't guarantee a Tormach can do it, but I believe it will. It will for sure come very close - you just might have to back off a bit on the depth. If you're having the tool pull out of the holder, or the holder pull out of the collet, then you don't have things tightened up adequately. I've been doing that cut with TTS for years on my knee mill, and never once had pull-out of any kind. In fact, I can stall the spindle without getting pull-out, and I have a 3HP motor.

Are you using the Tormach drawbar? If so, that is probably why you are seeing pull-out. You need to re-adjust it to put more tension on the drawbar. Your machine is capable of FAR more aggressive cuts than you seem to be using. In fact, my little X2 could easily do the cut you describe. What does your spindle power meter show when doing that cut? I'm guessing it will be quite low in the green. I calculate it at only about 0.2HP.

Regards,
Ray L.

[BAMCNC.COM]

Great post Ray!

[spork]

Can you draw a sketch on a piece of paper, scan it and post it here?

Will do. It will be pretty rough, but should give you the idea.

If you can, great. Let us give you a helping hand. I can't speak for the others, but I love to help out, up to and including showing you how to do some programming, or even making a couple of programs for you.

I really appreciate it. Everyone seems extremely helpful here.

Where do you live? I live in San Clemente, CA.

I'm in Mountain View - about 40 miles south of San Francisco.

If you send me a PM, I'll send you my phone number and we can talk about what you're trying to accomplish.

Done. Thanks.

What I specified is barely a 1HP cut. I can't guarantee a Tormach can do it, but I believe it will.

I believe I'll be using the Tormach 1100 with a 1.5 H.P. spindle motor.

Thanks again guys.

[SCzEngrgGroup]

I'm in Mountain View - about 40 miles south of San Francisco.

Practically a neighbor - I'm in the Santa Cruz mountains above Boulder Creek.

Regards,
Ray L.

[keithmcelhinney]

I don't have a Tormach (someday) and run a Novakon 135. I always read up on the Tormach pages because I am hoping to upgrade sometime this year. I am a complete novice so I ran my speeds and feeds on what people suggested on the Novakon forum. I usually use an 1/4" 3fl carbide endmill at .05-.07 doc with full width cuts at 13ipm and 3500rpm. I just went downstairs and ran a part with 19ipm (I am a bit of a wimp). I thought my it would run like crap but it ran much better! My chips were much better size and chip evacuation was way better. I was of the belief I was babying my mill but I think I was actually doing more damage to it. Spindle did not slow or stall at all.

HimyKabibble thanks alot! I am going to play with it more when I don't have paying parts to make. One thing to that I would love to hear your thoughts on is how to calculate speeds when you have to do a deep cut (I have one part that I cut with a 3/8" bit and I have to go 2.25" deep).

Thanks again!
-Keith

[SCzEngrgGroup]

I don't have a Tormach (someday) and run a Novakon 135. I always read up on the Tormach pages because I am hoping to upgrade sometime this year. I am a complete novice so I ran my speeds and feeds on what people suggested on the Novakon forum. I usually use an 1/4" 3fl carbide endmill at .05-.07 doc with full width cuts at 13ipm and 3500rpm. I just went downstairs and ran a part with 19ipm (I am a bit of a wimp). I thought my it would run like crap but it ran much better! My chips were much better size and chip evacuation was way better. I was of the belief I was babying my mill but I think I was actually doing more damage to it. Spindle did not slow or stall at all.

HimyKabibble thanks alot! I am going to play with it more when I don't have paying parts to make. One thing to that I would love to hear your thoughts on is how to calculate speeds when you have to do a deep cut (I have one part that I cut with a 3/8" bit and I have to go 2.25" deep).

Thanks again!
-Keith

With a 1/4" 3-flute carbide, you should be running up around 50IPM at that DOC. Ideally, you'd be running up around 7,000 RPM and 100 IPM. Even at that, it's only about a 0.4HP cut, so if you have at least a 3/4HP motor, you should be able to do it. Really, though, on these small machines, you're much better off using HSS - You can get the same MRR and you'll spend a LOT less on tooling.

On very deep cuts, you have to use a VERY "shallow" width of cut, to avoid the tool flexing. With a 3/8" tool at 2.25", assuming that too is a carbide 3-flute, I would try about 1800 RPM, 20 IPM, but you'll have to try both higher and lower values to find something that works, and avoids chatter. Such deep cuts are difficult. I wouldn't try more than a few thou width, probably 0.005" max, if not less. Certainly, for final finishing, you'll have to take several passes at no more than 0.001". If you get chatter (a loud "squealing" sound, reduce RPM, but watch out for tool flex as the chipload increases, as it can break the tool. Surface finish will degrade rapidly if you're pushing too hard. The only way to find the ideal parameters is to make lots of test cuts, and see what works best for your machine. Also, make sure you're climb milling. If you have ANY backlash, you'll probably have problems. And spindle or toolholder runout will really beat the he11 out of the tool, so make sure that is minimized as well.

Regards,
Ray L.

[spork]

On very deep cuts, you have to use a VERY "shallow" width of cut, to avoid the tool flexing.

Chiming back in with a stupid question if I may... I will be making some deep cuts (~1") but I figured I'd just do several passes of shallow cuts at full tool width. Yes?

Incidentally, I don't anticipate doing any finish pass. This thing is hidden from sight and precise dimensions are not critical.

[SCzEngrgGroup]

Chiming back in with a stupid question if I may... I will be making some deep cuts (~1") but I figured I'd just do several passes of shallow cuts at full tool width. Yes?

Incidentally, I don't anticipate doing any finish pass. This thing is hidden from sight and precise dimensions are not critical.

Yes, you will generally get maximum MRR (Material Removal Rate) running the tool full width, with depth equal to 0.5-1.0X the tool diameter, making multiple passes to reach target depth.

Finish cuts are generally either for reaching precise dimension, or just cosmetic, so you can leave them out if you like.

Regards,
Ray L.

[Moggot]

Steve,

What I specified is barely a 1HP cut. I can't guarantee a Tormach can do it, but I believe it will.
Regards,
Ray L.

For slotting with a 1/2" cutter .200 deep GWizard is suggesting more like 4000 RPM and 30IPM for about .6hp, but that's depending a lot on cutter type, length and how aggressive you want to get. As you said earlier, experimentation is key, but this is a pretty reasonable starting point.

The 1100 has a lot more umph then most think. When it comes to shaving time off a program my courage to go faster usually runs out long before the spindle runs out of HP.

[SCzEngrgGroup]

For slotting with a 1/2" cutter .200 deep GWizard is suggesting more like 4000 RPM and 30IPM for about .6hp, but that's depending a lot on cutter type, length and how aggressive you want to get. As you said earlier, experimentation is key, but this is a pretty reasonable starting point.

The 1100 has a lot more umph then most think. When it comes to shaving time off a program my courage to go faster usually runs out long before the spindle runs out of HP.

Power estimates are rather speculative, so different calculators will give different results, depending on what assumptions are made. However, 0.6HP seem way low to me, unles perhaps that is the power at the tool edge, rather than at the spindle motor? But, in any case, it is a cut many benchtop machines can make with little difficulty, and certainly not anything close to 20HP. With 20HP, we'd be able to run a good carbide 3-flute at over 1/2" depth, and over 100IPM, with plenty of power to spare.

Regards,
Ray L.

[spork]

Sorry for the delay guys. Here's a really awful sketch of the clutch adapter plate I'm planning to mill from 6061-T6 aluminum.

From memory, it's about 3" diameter and 1" thick. The three holes go all the way through. I figured I'd chock up a block of aluminum, mill the top surface to form the dogs, then mill the three holes, and finally mill the outline of the part in several passes, leaving some relatively thin tabs at the bottom to hold it in place in the block.

Am I thinking along the right lines?

Thanks again.

[Steve Seebold]

Sorry for the delay guys. Here's a really awful sketch of the clutch adapter plate I'm planning to mill from 6061-T6 aluminum.

From memory, it's about 3" diameter and 1" thick. The three holes go all the way through. I figured I'd chock up a block of aluminum, mill the top surface to form the dogs, then mill the three holes, and finally mill the outline of the part in several passes, leaving some relatively thin tabs at the bottom to hold it in place in the block.

Am I thinking along the right lines?

Thanks again.

You're close. I would start with a piece of material 1/4 to 1/2 inch thicker than your finished part. run the part complete on one side then flip it over and cut the back side off.

[David Bord]

Great post Ray!

+1

Ray, very very cool of you to take the time to explain in such detail.

I used to live very close to you... Beautiful area!

Not long after I moved, the house was shaken off its foundation by Loma Prieta.

David