endmills breaking, and feedrate

[SmaDoc]

I've been having problems with breaking the end mills I'm using. So I guess this isn't exactly a Mastercam issue, but I figured I'd try to run this by everyone neways. Originally I was using 1/8" dia 2flute endmills. The first 2 had a cut length of less than 1/4" I believe. After breaking 2 of those, I bought 2 more, with a 3/4" cut length. The deepest I would be cutting with these would be 0.6", which is why the 1st 2 broke I guess. Both the new endmills broke at the same point in a pocketing opperation, most likely because I dont know the proper feedrates for these size end mills. The stock I'm cutting into is 6061 aluminium. I started off with depth cuts of .015, and got rid of the rapid traverse commands (because it seems to cause loss of position on the LightMachine TMC1000 that I'm using, when it did use rapid traverse, every now and then you could notice a stair step starting to show, the part kept getting moved over just slightly, which I also found out was caused by having the feedrate too low. The estimated completion time for the part at this point was about 3 hours. I doubled the feed rate and depth of cut (depth of cut to .025), then the time for completion came down to just under 2 hours. Ran the program, everything was fine for about 90mins, and on the 2nd pass of a pocketing opperaiton the 1st bit that I bought broke. Figured it was because of the feed rate being too fast, so I took it down from 24ipm to 12ipm and got rid of the operations that were already completed, ran it again, and the 2nd one broke. So now I'm stepping up to a 2flute 3/16" dia end mill. Don't remember what the settings are on it at the moment, but tommorrow I'll be running it and seeing what happens. If i remember correctly I got it set at a depth of cut of .018 and I think the feedrate is now 14ipm, but I could be wrong. As far as RPM goes, I blieve its been over 3000rpm the whole time, which seems pretty fast, but all the stuff i've done so far all I know about CNc machining I've basicly figured out on my own, so, maybe I'm missing something here. If you like, below is a rendered picture of what the part should look like when its cut out. I'm working on making brake calipers for the Electrathon cars that I'm envolved with. The way I've come up with making them is to machine one side, flip the part around, machine the other side, and the part should fall right out, but I haven't gotten that far along so I don't know if its going to work yet. Any ideas, questions, or suggestions are welcome.

Thanks,

Sam

 

http://68.205.140.9:84/cad/brakes/caliper_inside_half.jpg

[J Coulston]

What type of collet are you using to hold the endmill?

 

Are they carbide or HSS end mills? Carbide is much stronger.

 

Are you using coolant? Is the broken mill flute packed with al? The al could be galling on the end mill.

 

I slot 6061 1/8 thick plates all the time with a 4fl carb stub em 6000rpm (max on my machine) 10.0 IPM 0.125 doc

 

Are you sure there are no colisions in the program?

 

If you are pocketing what type of entry are you using? Try a helix entry, or drill a pilot hole.

[Chris Rizzo]

quote:

---

The way I've come up with making them is to machine one side, flip the part around, machine the other side, and the part should fall right out, but I haven't gotten that far along so I don't know if its going to work yet. Any ideas, questions, or suggestions are welcome.

---

Acutally, holding the material and having the desired part drop out will invariably f-up the part. It will never drop "clean" out, without getting nicked/gouged/chewed by the cutter. Better option is to cut some quick softjaws the shape of your part and hold onto it..and hog off the excess material.

 

Also, 3000 rpm will work, but it's not enough. Whatever your machine has for max. RPM, run it. In 6061, I run everything 1" and under at 6000rpm.

[MACHINEMASTERG]

quote:

---

Are you using coolant? Is the broken mill flute packed with al? The al could be galling on the end mill.

 

---

+1

[Teh Bear without Brains kinda idiot]

---

cutally, holding the material and having the desired part drop out will invariably f-up the part. It will never drop "clean" out, without getting nicked/gouged/chewed by the cutter.

---

Not never .

The way to safely drop part is this

:

cut it through ,leave one or more tabs .

then take a plastic hammer and with a couple of light strokes break tabs ,or with sharp tool

or with last separate tollpath cut out cut teh tabs ,but direction of cutting must be conventional to falling part ,the mill will pull it out, not to push in .

I `ve done that a lot of times

 

HTH

WTHH

[Guest CNC Apps Guy 1]

6061 is horible stuff. Gummy, yuck! I'd go with a 3 flute or 4 flute. The rigidity just is not there with 2 because of the decreased IC down the shank. When I cut with them I usually run max RPM (10k) and about 16 IPM with about a .06 DOC. Also, get the shortest LOC yu can get, and oh, one more thing, use Solid Carbide. HSS is crap.

 

HTH

[Teh Bear without Brains kinda idiot]

Yes ,+1000 to James for all he says .

I say that with Iscar 3 mm mill with coating and strong enough short cutting leght ,the rigid setup I would go even faster(twice ,JMHO) .

But check your toolig ,get rid of radial bitting as much as possible .

And a lotof fluid .

If I would go with highspeed tools (Let`s suppose ) I also would go s5000 at least .

Also if you broke your tools at the corners of uour part drill them with drill or with end mill before making contour or pocketing .

Use hog mills as much as possible (solid hog mills rock ) .

Put your part on FTP to have alook on it.

HTH

WTHH

[robk]

quote:

---

HSS is crap.

---

+1

Does anyone still buy HSS tools for metal cutting? If you want to make the money, you have to spend the money up front to be competetive. Time is money.

 

quote:

---

Also if you broke your tools at the corners of uour part drill them with drill or with end mill before making contour or pocketing .

---

+1

I always pre-drill the corners whenever possible.

[SmaDoc]

Thanks for all the great ideas! J Coulston, the collet I'm using, not sure of the exact name but they have 3 slots on the end mill side, and a threaded "boss" at the other end, and when the bolt is tightened at the top it draws the collet up, thus compressing the collet around the tool. As far as letting the part fall out, I've done it before in machinable wax, but usually I stop it as soon as i start to see daylight through whats left of the stock, then just break it out and file any edges. Not using coolent (dont have a pump system :-/...the school was cheep when they purchased the machines. Luckily we have the Lightmachine mill other wise id be stuck with trying to use our Denford novamill *shudders*. As far as I recall with the 1st 2 bits that broke, they were carbide, I could be wrong though. Also the first bit that broke did have a little bit of alu built up in the flutes, but that was because I left it running and went to help a kid with something, not thinking to check on it offten enough because I had doubled the feedrate from previous feedrates (which got rid of the "stairstep" problem) but just as I got back and started blowing the chips out of the part...I was too late, too many chips built up and it broke. I'll try changing the spindle speed and see how that helps, also I'm now using a 3/16" bit instead, which will help cut down the part time somewhat, and its bigger so it SHOULD be able to stand up a little bit more to the forces plus lowering the feedrate should help also. I'll try to upload the mc9 file here shortly. If this works it will be my 2nd part that I've made successfully, the other was just a simple box with tabs and a pocket cut in the middle. Again thanks for all the help and ideas!

[Teh Bear without Brains kinda idiot]

If no coolant ,then I would use HSS tools

I will put on the part kerosine and will do it from time to time during milling and will blew chips with air .

Put your glasses on

[SmaDoc]

Hehe Yeah, glasses are a must, I'm always having to yell at the students to put glasses on. We have signs posted everywhere that say safty glasses are required in this area, but they just don't seem to care. I'm having problems connecting to the FTP from here at work. I'll keep trying but its most likely a "security issue" lol. I'll post it when I get home if I can't get it up from here.

[Teh Bear without Brains kinda idiot]

Have you tried kerosine on alluminium ,Smadoc !

 

Try it .

[Harryman]

Can you run a mist unit for cutting lube? Anything is better than dry in this application. Spray bottle if you must.

quote:

---

but just as I got back and started blowing the chips out of the part...I was too late, too many chips built up and it broke.

---

It only takes 2 seconds to have too many chips. They need to be removed constantly. Spray bottle in one hand and air hose in other.

[MetalMarvels]

+1000 to James also on the 3-4 flute stub tools in 1/8 and 3/16 diameters. If you can't flood coolant or even brush some coolant on it - an air blast (away from the operator at a low CFM) will help somewhat.

 

Sounds like you are using an R8 collet from your description - which probably means an open (unguarded) ops area - like with a knee mill. A mag-base shield in front of the vise would probably help you keep chips off the operators (I think that the shield might actually be an OSHA thing - but don't quote me on that - I will try to locate the reg - we have it aroung here somewhere.....).

 

+1000 on the 6000 RPM or better for that size tool - but if you aren't getting the chips cleared out of the cutting area - it won't matter - the tools will just break off when the flutes pack up with chips (slagged aluminum).

 

On those size tools, I will usually get a short LOC and relief grind the shaft 0.001-0.005 undersize to reach deeper without rubbing the side walls. I find that I get a much better finish than with a tool with a longer LOC - the relief ground tool is stiffer. I rarely use an 1/8 inch diameter tool with more than about 3/16 LOC.

 

+1000 to the PoohBear - I leave 0.002-0.005 of "tab" and just break the part loose from the "foil" that is left. This is usually only good (for me) for fairly small parts. Otherwise, I run the softjaw pocket arrangement.

 

Like the others, I generally reserve my HSS tools for playing in plastic.

[Fralex_francois]

quote:

---

Have you tried kerosine on alluminium

---

Nope...

What is it supposed to do??

[Guest CNC Apps Guy 1]

quote:

---

...What is it supposed to do??...

---

It's a great lubricant in non flood applications. It has a relatively high flash point, still not a good idea to smoke around it though.

[MetalMarvels]

A little "smelly" too - but it does pretty much stay put while machining. However, I prefer the Monroe Fluids Cool-Tool II - it smells MUCH nicer and works even better than kerosene. The "spec" sheet is here: http://www.chess.cornell.edu/Safety/MSDS/cool_tool_II.htm

[Fralex_francois]

Are you serious you machine with this stuff, and doesn't goes on fire??

[Teh Bear without Brains kinda idiot]

Run many times .

[Guest CNC Apps Guy 1]

Note the high flash point. It's still flammable but when used with care in Non Ferrous metals, you're pretty safe machining with it. Yeah it is smelly though.

 

James teh lived to tell about it.

[MetalMarvels]

If you take the kerosene and cut it about 50/50 with a high sulfur content oil - the old boys used to use that for cutting steel. Smoky, but it works. Probably carcenogenic as heck too.....

[Guest CNC Apps Guy 1]

LOL!!! I just prefer not to think about the carcinogens and accept it as a cost of doing the job. Don;t get me wrong, I still take the precautions necessary to be safe but there's still an element of assumed risk in our jobs.

[Tim Johnson]

Any type of lubricant is better than dry. Go to a department store and get a $1.00 sqirtgun and use it with soapy water if you have to. Typically you would feed at .001 per flute, but at 3000 rpm you should be able to feed at .002 at .06 deep. (12 ipm for two flute)

[SmaDoc]

Well, I went the route of using a spray bottle with adjustable nozzle, spent all day with it lol, cleaning the chips out every now and then. I'm thinking of maybe looking for a pump or something on ebay, just to see whats out there, and look'n around else where. If I'm not mistaken the TMC1000 we have does have an output for a coolant pump, but I'm not sure. It'll go all over the place, but with the gaurd up it'll help somewhat by keeping everything confined. The only problem I have now is that it was starting to loose its possitions, every step in the path would be off by about .001 or less, and since it was getting close to the end of the day I just decided to stop it and start working on it again next week, after the hurricane (assuming the school/machine area is still ok lol, I'm sure it will be though). I'll try to upload the mc9 file to the ftp for those interested in looking at it/givign me any ideas (being as that I'm a "noob" at machining, I'm sure some improvements could be made. Thanks again for all the help and support!

[SmaDoc]

Ok I have the mc9 file uploaded now on the ftp its in the mastercam_forum mc9 folder, the filename is CALIPER_INSIDE_HALF_2.MC9 I'm not sure how close that is to the file/tool paths that I used today, but it SHOULD be pretty close to the same. If I would have thought about it before I left the school I would have taken a picture of what I did accomplish today, but oh well, thats how things go sometime. Atleast the bit didn't break this time(but I did use a 3/16 bit.