Hoss, hello and many thanks for your most constructive reply.Originally Posted by hoss2006
Well I can see where I went wrong as I used the same S & F calculator as you have.
However I used a Chip load of 0.1397 which I guess is just way too large as it is ten times the value you have used hence the broken tool and poor cutting.
Basically what I used was data from the form the link below
http://www.pdscolombo.com/spindle_speed.htm
I then took the mean and minimum Aluminium values to produce what I thought was a reasonable way to arrive at a Chip Load and then converted this to mm.
Thus ((0.002+0.009)/2)*25.4 = 0.1397.
So you see I have tried to understand, but I have either mist understood something or have used some over optimistic Chip Load data from the above web site.
Again many thanks for you input and well if you have a link to some GOOD materials chip load data then it would be really appreciated. (At this time I think I will only be working in plastics and soft metals)
IMK
Best to start using the lowest number if they give a range to be safe.
You could incorporate the chip load into your program by taking their material selection and tool dia. and
compare it to one of the charts to output the speed/feed so the user wouldn't have to input it.
Still these are just some general guidelines to follow as actual chip load is tool manufacturer specific, usually higher.
It'll get you going but as has been said, experience will be you best teacher.
Good luck, Hoss
Last edited by hoss2006; 06-28-2009 at 04:25 PM.
Gosh, you've... really got some nice toys here. - Roy Batty -- [URL]http://www.g0704.com[/URL]
Hello again Hoss and many thanks for your input.
So I shall try out the new feed rate tomorrow to see how it goes and let you know.
So was just wondering if you had recommendations for Plunge Rate, and Depth of Cut per pass please.
Have a good evening IMK
For plunge rate, use 1/2 the feed rate. For depth of cut, start at 1/2 the tool diameter, then go deeper if your machine, and the tool, allow it. If you push too hard, surface finish will go to hell in a hurry. Use that as your cue to back off. For chipload, try to stay near the maximum - it's a lot easier on the tool. Reduce RPM if necessary to keep it there. Too much RPM, or too little chipload will both cause the tool to heat up. When you get it right, the tool stays cool, and the heat gets carried away in the chips. If the tool is getting hot enough that you have chips welding to it and clogging it, and/or the chips are NOT coming off HOT, you're probably doing something wrong. You will also be severely limited in what you can do without some form of coolant. Mist works very well, with virtually no mess.
Regards,
Ray L.
BTW - Depth of cut is determined mostly by the rigidly and spindle power of your machine. Generally, if your goal is removing material quickly, you want to go as deep as the machine will allow. On most benchtop machines, that won't be very deep. At some point, you may have to back off, if you either can't keep the chips clear, or can't get enough coolant in to prevent burnign or welding. But other than that, DOC is pretty much independant of RPM and chipload. Pick your RPM, based on SFPM (80-100 for mild steel, 300-400 for aluminum, if using HSS tools). Then pick your chipload, based on the tool makers recommendations. If you get poor surface finish, or the machine shakes and "complains", reduce RPM, but maintain the chipload, until the machine is happy. A reasonable "rule of thumb" for chip load is figure 0.002" for a 1/2" tool, and scale by tool size for larger or smaller tools. So, for example, a 1" tool would give 0.004" chipload, while a 1/4" tool would give a 0.001" chipload. Below about 1/8", you need to get more conservative, or you'll break a lot of tools. Once you have the RPM and chipload happy, then see how deep you can go. Again, when you see surface finish deteriorate, or get shaking or the spindle slowing down, back off.
Regards,
Ray L.
I can see where you can get confused when so much misinformation is posted.
For Plunge Rate 25-50% of the milling rate is typical. DOC is as I've said is machine specific.
As with chip load, start conservative and work your way up.
A DOC 25% of the tool diameter is a starting point.
The extended length of the endmill in your pic would also reduce the force it could handle.
The .001 (.025mm) chip load is recommended as a starting point on chart after chart.
Harvey Tool has a troubleshooting guide for carbide endmills.
As they note, a cause of a many of the troubles like you've experienced are from too high a chip load i.e. feedrate.
Start conservative and work up to aggressive.
Good luck,Hoss
Gosh, you've... really got some nice toys here. - Roy Batty -- [URL]http://www.g0704.com[/URL]
conical tapered carbide endmill feed and speed calculations-
searched the web for a good 2+ hours and am still as lost as before
any ideas?
These 2 pages have some tips to follow for speed and feed.
Bits and Bits
Antares Inc
Hoss
Gosh, you've... really got some nice toys here. - Roy Batty -- [URL]http://www.g0704.com[/URL]
In the absence of concrete info I would use the major diameter of the cut for the speed calc and the minor diameter of the cut for feed. DOC etc. will be suck it and see.
Phil
feeds and speed?
honestly I say follow your basic formulas, and throw some stock in a (manual) mill ( THE REAL ONES ) and practice practice pratice, thats where the term "tricks of the trade come from", just remember fast feed slow rpms hogs chips, and slow speed fast rpm finishes. other than that like i said above , practice.
but curious did you ever complete your program?
Thanks Ray,
That is great advice for a newb like myself. I never could get an explanation of how DOC is related to chip loading etc, but this makes perfect sense of how to proceed. I think I've found pretty much every method to break an end mill over the last couple years. When I started this I though it would be way simpler than it is. I have a huge respect for machinist that know what they are doing. I've made a lot of parts since I got the machine (2-1/2 axis), but they looked like crap (surface finish etc.) After digesting all the different information on speeds and feeds, this thread tied it all together. I realized I was working the tool/machine way too hard. Way too low chipload/ too high RPM was heating the tool so much as to cause steam to come out of the cooling fluid ( I can hear the laughing ). I slowed the RPM and increased the feed rate for roughing, and payed a lot closer attention to MFR chip load recommendations (Duh), and the machine is working half as hard without all the "drama". My finishing passes look 100 times better as well.
Here's my last setup that worked really well (compared to before). Feel free to further advise-poke holes etc.
Material:6061 aluminum
Roughing 2100 RPM (3000 max ) feed 30"/min(max)
Roughing end mill 3/8" Destiny 3 flute "diamond back" recommended CL .006
Max DOC .3" ( I don't have a way to know the actual RPM under load and I'm too scared to go any deeper)
Finishing: 3000 RPM @ 16"/min full DOC "profile cut" .016 left on wall from roughing.
finishing end mill: 3/8" Destiny Viper
I played with different feed rates on finishing from 16"/min down to 8. Can't really detect much difference by "look or feel".
One Question if you don't mind.
How does chip load relate to # of flutes ?. I noticed this #changes in HSMworks as I change the # of flutes. Is the recommended CL per tooth (flute) ? or the sum of all flutes combined ?.
Thanks again for the great info.
Matt
Mill CNC Masters CNC jr.
Software Solidworks/HSMworks.
Those numbers are pretty reasonable. The most important thing is the result. If you're getting good finish, and not heating up the tool, then you're OK. Keep in mind for smaller tools, you need to reduce the chipload, for larger tools you can increase it. It scales pretty much with diameter, until you get below about 1/8", at which point the tools become rather more delicate, so chiploads have to be reduced further. In general, as tool diameter decreases, RPM should increase more or less linearly, and chipload should decrease more or less linearly, leaving the feedrate about the same. When you get the RPM, depth, and feedrate right, you can hear the difference - it just becomes very smooth and quiet. If you start getting a lot of heat, or the tool clogs, you're most likely feeding too slowly, or RPMs are too high. If you're breaking tools, other than due to chip welding, probably your chipload is too high.
Chipload is normally (not always!) expressed as feed per tooth, so doubling the number of flutes means you double the feedrate. For aluminum, stick to 2 or 3 flutes for roughing, and 4 for finishing. 4-flutes will tend to clog up when roughing, because there just isn't enough space to get the chips out.
Regards,
Ray L.
IMK
I think it may be helpful for you to understand the job, you are attempting to take on.
The varibles do not end at tool and material. Length of cut, interuptions, machine variables like stiffness of the tool/machine combination all effect tool life and tool effectiveness.
That would be one very useful program.
The closest single source - Sanvik's tool catologue.
Please post your program-I'd like to try it.
There is a program call ME Consultant you can try. They have a free (old) version and trial versions of current issue available. The trial versions are here: Close Tolerance Software . You can Google for the free version, as I don't recall where I got it.
I have found ME Consultant to be quite helpful, especially as a starting place.
I figured I'd ask this here instead of making a new thread as it relates. I'm cutting some heatsink fins in 6061 and am trying to figure out why my finish looks like it does. The slots are .144" wide, the endmill is a .125" and the gcode has it ramp down and then go around the perimeter on each pass. Final clean up run is .001" on sides and depth.
The problem seems to be on the ~.01" on each side of the slot it removes after the slot. It tends to screech a little depending on the rpm and feed rate but it doesn't make sense to me. As it gets farther into the hole it gets worse.
Maintaining the same chipload of .001 I get:
4200rpm - best finish and minimal screech
6700rpm - worse finish, kind of ripply and most screech
106000rpm - middle finish, slightly more screech than 4200 and much less than 6700
Why is it that 6700 gives a worse finish that 10k and how do I get a better finish? I tried increasing the feedrate when it's cutting the perimeter because of chip thinning but it just makes the screeching worse. I'm using flood coolant and removes the chips quite well.
How deep are you cutting? Screeching is usually due to the work vibrating, and speeds that have the cutter teeth hitting at near the natural frequency of the piece will make the screeching worse. If so, the only solution is to make shallower cuts, so you don't deflect the work so much.
Regards,
Ray L.
I think it's a vibration problem like you mentioned. Original DOC was 1mm and I just tried .8mm and got the same results. I sat another toolmakers vise on the table while it ran and the finish got better. I have some rubber/cork dampers between my enclosure and the table and I think they may be causing this.
Reply with Quote
