[binfordw]

Hi,

I've had time the past few days to spend with my X3 again, and have been working on a few projects. Some questions popped up.

First, Feedrates. I still dont really know what Im doing here. With 3/8"-1/2" endmills its not a big deal really, I can listen and adjust accordingly, but the jobs I ran lately used a .187" endmill and I found I had to run at painfully slow feedrates (4-7ipm) to feel "safe"

How do I tell what feedrates a bit will safely cut at a set rpm?


Also, I'm interested in getting some plastics to mess with, but the last website I searched for prices, it all seemed higher than aluminum. Since theres 400 different types of plastic, what is a commonly used type for general machining?


Thanks in advance for any help!

Ben W

[SCzEngrgGroup]

RPM is determined by tool diameter, and material, by calculating SFPM - Surface Feet Per Minute as follows:

SFPM = (PI * ToolDiameter * RPM) / 12 or,

RPM = (SFPM * 12) / (PI * ToolDiameter)

This is usually rounded to:

RPM = SFPM * 4 / ToolDiameter

SFPM is a function of the tool material and the work material. For mild steel being cut with HSS cutters, SFPM should be around 80. For aluminum, 400 SFPM is a good average. If using carbide, double or triple those numbers. So, if you're cutting mild steel with a 1/2" HSS endmill:

RPM = (80 * 4) / 0.5 = 320 / 0.5 = 640 RPM

Feed rate is a function of RPM, the number of flutes on the tool, and the "chip load", which is the nominal thickness of the chip each tooth carves out:

FEED(in IPM) = RPM * #Flutes * ChipLoad

Chipload is a function cutter diameter, and for roughing cuts ranges from perhaps 0.0004" for very small endmills (1/16") to perhaps 0.008-0.012" for large ones (1"), and varies more or less linearly for sizes in between. So, for a 1/2" 4-flute endmill, assume a 0.004" chipload, and you get:

FEED = 640 * 4 * 0.004 = 10.2 IPM

Depth of cut should be as much as you can get away with, which will be limited by spindle power, machine rigidity, and coolant used.

Now, you're not likely to reach this numbers on a small mill, due to the limited spindle power, limited rigidity, and inadequate cooling. So, start by setting the calculated RPM, pick what you feel is reasonably modest depth of cut, and start by feeding at perhaps half the calculated rate. Increase feed rate until finish quality starts to degrade. When you reach that point, back off on the feed rate perhaps 10%. Now increase depth of cut until the machine starts shaking, or the spindle motor starts laboring, then back off a bit.

There are no canned numbers, as every job is different, and you have to learn how to "read" the machine. Some rules of thumb:

Keep chip load as high as possible. If you find you have to reduce feed rate well below the calculated value, then reduce the RPM to keep the calculated and actual feed rates reasonably close. Running high RPM with low chip load will cook tools faster than anything.

Here are some typical numbers I use on my mill:

1/2" 2-flute HSS endmill, 6061 aluminum: 3100 RPM, 30 IPM, 0.125" DOC
1/8" 2-flute HSS endmill, 6061 aluminum: 8000 RPM, 12 IPM, 0.125" DOC

With limited spindle speed, 4-7 IPM is probably about all you can do with small cutters.

Regards,
Ray L.

[binfordw]

So the chipload is a rough estimate for tool sizes? The charts I found where I get my endmills list chiploads under like, 1/8", 1/4", 1/2", 1". So I use the closest to what tool Dia. Im actually using?

The job I cut today was a .187" 2 flute endmill, 2k rpm, 6 ipm. It did not seem to like that much.

When I calculated things, it looks like the SFPM was around 100, when the Alum calls for alot more. Although I'm not exactly sure- roughly bits list 150-400 sfpm, another says 600-1200 sfpm.


I ordered the gears and belt to change my X3 over to a 0-6k rpm spindle speed, I hope that will help things. Running a 3 flute high helix .187" endmill at 6k rpm I'd sure like to get 15-20ipm feeds.

[SCzEngrgGroup]

So the chipload is a rough estimate for tool sizes? The charts I found where I get my endmills list chiploads under like, 1/8", 1/4", 1/2", 1". So I use the closest to what tool Dia. Im actually using?

The job I cut today was a .187" 2 flute endmill, 2k rpm, 6 ipm. It did not seem to like that much.

When I calculated things, it looks like the SFPM was around 100, when the Alum calls for alot more. Although I'm not exactly sure- roughly bits list 150-400 sfpm, another says 600-1200 sfpm.


I ordered the gears and belt to change my X3 over to a 0-6k rpm spindle speed, I hope that will help things. Running a 3 flute high helix .187" endmill at 6k rpm I'd sure like to get 15-20ipm feeds.

With small bits, you MUST use coolant, or at least a strong blast of air, to keep the chips clear.

Regards,
Ray L.

[ronncat]

Ben,
Care to elaborate on the belts and pulleys you ordered. I am considering increasing my spindle speed as well now that I am making chips. Thanks.

[binfordw]

Sure, I got the info from another CNCzone member. I just got mine installed, it does take a little work, you have to bore the small pulley out to fit, technically you need to cut a keyway in it too, but I just used the setscrews in the keyway groove on shaft. With the gear reduction between it and the spindle I dont think it will have too much force on it to really need the keyway. I bored mine to be a really snug fit, that'll help too I suppose.


Go Here - https://sdp-si.com/eStore/Direct.asp?GroupID=346

And enter these numbers to find the parts (Include the A)

A 6R55M082150 (Belt)

A 6A55M032DF1512 (Large pulley)

A 6A55M019DF1506 (Small pulley)

The belt might not be a neccessity, it seemed to be the same length as the one I took off. Probably good to use a new one on the new gears though I guess.


I stuck in a 1/8" 2 flute and did some quick test cuts in alum, it really FLYS now, Im very happy. Before the swap I had just cut an alum job with a .187 endmill, that I was stuck around 5-7ipm feedrates. Painfully slow, took hours to complete. During my test I was cutting .05" deep passes with the .125" bit, up to 30ipm without even having the spindle speed maxed out. 30ipm is smoking fast compared to 7! lol. Im going to tweak my program a bit and try the parts again with the new speeds to see how things go.

[binfordw]

Well two broken endmills later, I'm still not up to speed on setting feedrates/spindle rpm apparently :/

I tried what I thought would be close, 4500 ish rpm, .187" 2 flute, 15ipm feedrate(with mist coolant). It started well, but after 4 or 5 pocket cuts in the program, it started to gall up. I stopped it, and the bit had alum sticking to the flutes. I cleaned it up and finished the program, but the bit was crap after that, it broke the tip of one flute off later as well.

When material welds to the flutes, that means the rpm is too high?

I've got 5 more good 3 flute endmills coming in the mail, hopefully I cant get a grasp on things before I break all of them too lol.


Anyone know anything about the plastics in my original post?

[ninefinger]

For a good all round "engineering" plastic I like acetal (Delrin is Duponts trade name). Quite strong and hard, slippery and machines nice. Good bushing / slider material. Racers use it as bushings on pivot points on car suspension, etc. Readily available too. Lots of colors to keep people interested!:rainfro:

For feeds and speeds try out Bob Warfields G-wizard http://cnccookbook.com/CCGWizard.html

Mike

[Teyber12]

bookmarked this thread..

[ronncat]

Ben,
Thanks for the reply. Your links however lead to the catalogue pages and not to specific pulleys and belts. Do you have the stock number or description for the items you used? Thanks again

[binfordw]

Guess I should have checked the links heh. I went back and edited the post, I stuck in the part numbers instead of the bad links.

Sorry!

[ronncat]

Thanks...I'll check it out!!

[binfordw]

Does Aluminum "welding" to flutes means the rpm is too high?

I think maybe the last 2flute bit I broke was because I had run several programs at a very slow feedrate and max rpm (was 2,000 at the time). It started to cut well at the settings I calculated, but threw in the towel after a few pockets and galled up with material. I do run "Kool mist" coolant during cutting.


When I get things cutting, Can I slowly back off the rpm until I can tell things are starting to strain, then set the rpm a little above that to prevent running at too high of rpm?

I used to slow the feedrate, but I dont feel like I should have to cut so slow now that I have access to the proper spindle speeds.


Can someone give me what settings they would use for a .187", 3 flute high helix endmill, cutting .050" per pass? I have it programmed to feed at 20ipm, I'll likely start at 50% to see how things go. I have replacement .187" bits that should be here today from Maritool and I'd like to not break them all by this evening

[SCzEngrgGroup]

Does Aluminum "welding" to flutes means the rpm is too high?

I think maybe the last 2flute bit I broke was because I had run several programs at a very slow feedrate and max rpm (was 2,000 at the time). It started to cut well at the settings I calculated, but threw in the towel after a few pockets and galled up with material. I do run "Kool mist" coolant during cutting.


When I get things cutting, Can I slowly back off the rpm until I can tell things are starting to strain, then set the rpm a little above that to prevent running at too high of rpm?

I used to slow the feedrate, but I dont feel like I should have to cut so slow now that I have access to the proper spindle speeds.


Can someone give me what settings they would use for a .187", 3 flute high helix endmill, cutting .050" per pass? I have it programmed to feed at 20ipm, I'll likely start at 50% to see how things go. I have replacement .187" bits that should be here today from Maritool and I'd like to not break them all by this evening

Welding indicates:

1) RPM is too high and/or
2) feedrate is too low and/or
3) you need to do something to keep chips clear of the tool and/or
4) coolant or lubricant is required

So, either reduce RPM, and/or increase feedrate, and/or add air, coolant or lubricant.

If RPM is too high relative to feedrate (i.e. - low chipload), heat will build up in the tool, rather than being carried away by the chips. Set RPM based on recommended SFPM for the tool and the material you're cutting. Calculate feedrate based on recommended chipload for the tool you're using. Start with shallow cuts, to make sure you're not over- or under- loading the tool. If all is well, then increase depth of cut until surface finish starts to degrade, then back off a little. With small tools, use a strong blast of air right on the tool to keep chips clear.

Regards,
Ray L.

[binfordw]

Thanks, that does help a bit. If I can bug you some more- A "whining" or resonating squeal, suggests too slow feedrate/ much too high rpm?

I thought I had things working well, the new bits were cutting great, but I got through a few parts and one broke.

Apparently I was trying to run too high a feedrate for the rpm (Correct?), roughly 3k-3300rpm at 16-17ipm or so(.187" 3 flute endmill). After it broke I slowed the feed a tad and upped the rpm a bit, and it sounded ok, and ran the part out fine.

I dont really know why Im struggling so much with calculating feedrates. I thought I could tell decently what "sounded" ok, but Im still damaging endmills, and its quickly getting frustrating and expensive. I think I may need to setup a tachometer to help me out, since after all I do have to guesstimate rpms pretty roughly.

[SCzEngrgGroup]

Funny noises are a function of the machine, and don't relate to anything in particular w.r.t. the RPM, feed, etc. They're the result of something loose in the machine, or a resonance in the machine. Changing RPM or feed up or down may, or may not, help, depending on the source of the noise.

Regards,
Ray L.

[binfordw]

I still need help with this..

I've been able to run .187" bits without breakage for a bit so far, but I tried some 1/16" and broke them. I tried G wizard, as well as using all the formulas necessary with no real help.

Chipload sees like a "guess" number. I don't understand how you figure the chipload, and since figuring feedrates require it, I dont think guessing is helpful.

As of right now, Im trying to get a program to run with a 1/16" endmill, I need to get this done for a class tuesday. I tried a 3 flute .0625 endmill, 6k rpm, 10IPM feed and at only like .030" per pass and it snapped off after a few passes. I have 2 or 3 4 flute 1/16"'s left, so Im going to try the program in steel. I guess I will cut the feedrate and hope to get through atleast one part.

I would like to be able to run 20-30 parts, but I'll really need proper settings to do so.