[mannymade]

@Ray - do you realize that you have just committed BLASPHEMY on this site? Every one here says that you need carbide/insert tooling for every thing on all machines. That HSS is worthless in todays world.

For high production volumes I agree.

[SCzEngrgGroup]

@Ray - do you realize that you have just committed BLASPHEMY on this site? Every one here says that you need carbide/insert tooling for every thing on all machines. That HSS is worthless in todays world.

Just wait. Someone will argue the point.....

Regards,
Ray L.

[mannymade]

Since I have a max RPM as well (1100/3000) I have to do the same correct?

Yes you'll have to. I have a mill with a 30 horse motor a travel of 76 inches X 48 inches Y and 30 inches Z. I have the option of a spindle increaser but just manipulating the speeds and feeds for me is enough.

[BobWarfield]

Just wait. Someone will argue the point.....

Regards,
Ray L.

Heh, heh, heh (Evil cackle)...

Funny old topic, this carbide vs HSS one.

There are performance envelopes where HSS can achieve a higher material removal rate than Carbide. Because it is less brittle, it typically has a higher chipload. Carbide takes a lower chipload but can achieve a much higher surface speed. HSS will win if your spindle can't go fast enough to offset carbide's lower chiploads.

To see a chart of this for aluminum, check out my article here:

Is Carbide Always Faster? « CNCCookbook

Ray's knee mill has a faster spindle than a lot of the hobby machines. My poor old IH mill is limited to a ridiculously low 1600 rpm, for example. But Ray's machine is slow too by today's VMC standards.

For a lot of machinists, I will contend that the limiting factor is not these chipload/rpm combinations, but tool rigidity. If you're using a tool less than 1/2" in diameter, it's a piece of wet spaghetti, rigidity-wise. It needs all the help it can get, and I advocate carbide for those cases because it is 3x as rigid as HSS. For 1/2" and up, see if your spindle and machine capabilities make carbide worthwhile. On less-than-VMC's, it frequently isn't worth the expense.

For larger indexable tooling, it's more a matter of convenience. Hobbyists can do fine with patience and a well ground HSS fly cutter. Pros need more productivity.

Another issue is for hobby machines your spindle runout. Since HSS is less brittle, it is more tolerant. I know machinists who swear by small carbide EM's and I know those who swear at them. The latter have enough runout they're breaking the little tools too easily.

As you can see, the short answer to all this is it depends. You have to run the numbers AND know your machine.

Nateman, the best way to get familiar with the numbers is to either use a calculator like G-Wizard or MEPRo, or build yourself a spreadsheet. G-Wizard started out as a big Excel spreadsheet until it got too complicated. You'll learn a lot putting together a spreadsheet.

The thing not to do is take the numbers for granted and assume a few simple rules of thumb will carry you. They may keep you out of trouble, but they won't produce the best results. The math is just too complex for that to work well!

(chair)

Cheers,

BW

[photomankc]

@Ray - do you realize that you have just committed BLASPHEMY on this site? Every one here says that you need carbide/insert tooling for every thing on all machines. That HSS is worthless in todays world.

No way, I love me my good HSS tools. Sharp HSS in Aluminum is a joy. However, when I do steel that's when it gets ugly with them. I am going to give solid carbide a try and see if I can save the HSS tools for the easier material.

Definitely keep the tool loaded up at 0.002" per tooth or more which means running the RPM that lets you do that as much as possible. I notice the great improvement that has come with CNC conversion and the fact that it doesn't slow down and rub the crap out of the tools trying to get to the right number on the hand-wheel. Finish looks good and my tools are staying sharp longer. But steel seems to burn up the corners on my HSS tools no matter how well I try to stick to the numbers. Lack of flood doesn't help I'm sure.

[SCzEngrgGroup]

No way, I love me my good HSS tools. Sharp HSS in Aluminum is a joy. However, when I do steel that's when it gets ugly with them. I am going to give solid carbide a try and see if I can save the HSS tools for the easier material.

Definitely keep the tool loaded up at 0.002" per tooth or more which means running the RPM that lets you do that as much as possible. I notice the great improvement that has come with CNC conversion and the fact that it doesn't slow down and rub the crap out of the tools trying to get to the right number on the hand-wheel. Finish looks good and my tools are staying sharp longer. But steel seems to burn up the corners on my HSS tools no matter how well I try to stick to the numbers. Lack of flood doesn't help I'm sure.

"Definitely keep the tool loaded up at 0.002" per tooth or more" - Making a statement like that without talking about what size tool you're referring to is a recipe for disaster. A 0.002" chipload is FAR too much for a 1/16" endmill, and FAR too little for a 1/2" endmill. Chipload is very much a function of the tool diameter, type and depth of cut, and the particular tool.

Regards,
Ray L.

[photomankc]

Point taken, but the OP is referring to a 3/8" tool not a 1/16" or 1/2". I can see it being easy to take wrong though so I'll say now that I'm referring to a 3/8" endmill on a small machine. I don't think you want to go much lower but you may be able to take more if the machine doesn't throw a fit over it.

My point is more that going in slow-mo is not being kind to the tools. You need a calc to start out with so you know about what the right load is so you aren't snapping tools or grinding things instead of cutting them. It's a bit overwhelming at first.


Sent from my iPod touch using Tapatalk

[nateman_doo]

I said, "what the hell..." and I ran my machine at 14ipm through the copper and it ate it up! I used athe 2 flute carbide bit that I used for calculations, and it worked perfectly. I do intend to pick up that RPM reader to get a more accurate reading, but I already cut 75% faster then before.

[SCzEngrgGroup]

I said, "what the hell..." and I ran my machine at 14ipm through the copper and it ate it up! I used athe 2 flute carbide bit that I used for calculations, and it worked perfectly. I do intend to pick up that RPM reader to get a more accurate reading, but I already cut 75% faster then before.

Knowing the exact RPM is of little practical value, and setting RPM precisely also is not worth much. You need to learn to "read" the cut, by looking at the resulting surfacer finish, and, most importantly, *listening* to the machine. When it's right, it *sounds* right - a nice, smooth, quiet hum. When it's wrong, it sounds bad - squealing, chattering, warbling, vibrating, and the surface finish suffers, and/or things break or bog down. Just pick your RPM (even if you're doing so half-blind), start with a shallow cut, get that working nicely, then start going deeper until things degrade. If your RPM is off by +/-20% or more, it won't make a bit of difference if you tune everything else accordingly. Your only loss will be a lower MRR if you end up at a lower than optimum RPM. If you're 20% high, it won't really have any significant negative impact if everything else is adjusted accordingly.

Regards,
Ray L.

[nateman_doo]

The fact that I can see the reflection of the machine means its a pretty decent cut right? The edges of the cut are kind of chattery, but I didn't program a finish pass into the work. I will save that for the outside edge.



That cut you see there initially took me around 2 hours to do at the 3ipm, now it took me 22 minutes @ 14 ipm, and 5 ipm on the sloped entrance cut.

[nateman_doo]

15-25 days to get that little RPM reader. Slow boat from China it seems

[error404]

I just found this thread.... and i get the feeling is going to come handy when my X2 is up and runing

15-25 days to get that little RPM reader. Slow boat from China it seems

(nuts)

[nateman_doo]

I am looking at the charts and making a quick reference guide for most of the bits that I use.

[error404]

The sfm figure will tell you what rpm to run at. It will be different depending on the diameter of the end mill you are using.

Milling Formula Calculator

Here is a calculator that is useful.

when using the calculator... is the Diameter in inches or mm?

[nateman_doo]

I would say inches.

[nateman_doo]

I made a feed & speed chart for the X2 motor. Do all of these numbers look good? I used lots of conservative numbers in the calculations.

[error404]

So... what happens when the RPMs are outside the X2 capabilities?
do you reduce the IPM? (BTW what's the maxium RPM on a X2?... 2,500?)

[nateman_doo]

I think 3K with that bolt on belt drive.

[TXFred]

So... what happens when the RPMs are outside the X2 capabilities?
do you reduce the IPM? (BTW what's the maxium RPM on a X2?... 2,500?)

Within reason, you can reduce RPM and reduce feedrate by the same factor in order to keep chip load the same.

Or you can switch to HSS, which likes to run at lower speeds than carbide. It also lasts better on chattery machines like X2's. Carbide does not like to chatter. If it does, it will chip.

By the way, here's a picture I took of two parts from work. These are steel parts that are turned on a lathe. The combination of steel and lathe is great for showing you when you have the wrong surface speed. This pic demonstrates why surface speed is so important.



The part on the left is an old part that was programmed at a spindle speed that is too slow. The outer edge of the part where the diameter is biggest looks OK, but as the tool moves inwards, the finish gets worse and worse because the surface speed is decreasing.

The part on the right is from my program. :banana: I increased the surface speed, and programmed constant surface speed, so the spindle sped up as the tool moved inwards.

Cheers,
Frederic

[error404]

Nice granite workbench!!!