LinkBack URL
About LinkBacks
Easier to help if you give more details.
Material, cutter diameter and type, speeds and feeds you are currently using.
Even what you are doing, could maybe done differently and more efficiently.
| | |
I'm trying to optimize the cutting parameters on my X3. From my limited experience so far DOC seems to be the "hardest" thing for my machine. In 6061 aluminum at a DOC of 0.05" I can run the machine at G-Wizards recommendations with zero problems. However at 0.1" DOC at G-Wizards recommendation, the entire machine shakes itself apart. This is true for both 1/2" and 3/8" cutters that I've tried. I've tried all types of geometries, 2 flutes, 4 flutes, 3 flute High Helix, 1 and 2 flute indexable. In all cases 0.05" DOC is easy and 0.1" and all the screws come loose on the machine from the shaking.
I'm to green to tell if it's a rigidity issue, chatter problem, or some other unknown issue.
I'm fine running at 0.05" DOC, I'm not really interested in super speed. However, intuitively my cutter life should be double a 0.1" DOC since I'm using twice as much cutting surface to perform the cut.
Some examples of my speeds and feeds: 3/8" 3 flute, aluminum specific endmill: 0.1" DOC full slot @ 18 IPM, conventional milling in 6061. Machine shook its ball screw mounts loose, and the gib screws backed out.
1/2" 1 flute APKT, 0.1" DOC full slot in 6061 at 14 IPM, conventional milling. Same result. All of these are using mist cooling. I tried climb milling as well with similar results.
Both above examples worked at 0.05" DOC flawlessly. Extremely smooth, and easy.
What kind of DOC in 6061 aluminum should I expect from an X3? Any tips for achieving greater DOC's so that I can maximize tool life?
-Jim
Last edited by Kingjamez; 10-24-2010 at 08:34 AM. Reason: add more details.
Easier to help if you give more details.
Material, cutter diameter and type, speeds and feeds you are currently using.
Even what you are doing, could maybe done differently and more efficiently.
Thanks for the suggestion, added more detail to the first post.
Ah RPM would be nice to know. Or is it a secret.
How/what are you cutting, a face, a slot/pocket, are the cutters new and sharp.
Are you using quality tooling ?
I'm running at the max speed for a X3: 2000 RPM.Originally Posted by M250cnc
Ah RPM would be nice to know. Or is it a secret.
How/what are you cutting, a face, a slot/pocket, are the cutters new and sharp.
Are you using quality tooling ?
I could be cutting anything, slots / pockets / profiles. I have lots of projects. In the above examples, I'm cutting slots.
The cutters are all new. Here is the 3/8" :3/8" Carbide Endmill 3F .030" Rad Alum Rough-Finisher - eBay (item 280548911840 end time Nov-12-10 12:27:41 PST)
The indexables use this insert: APET 1003 PDER - MP3 FOR ALUMINUM. FITS APKT HOLDERS - eBay (item 260505643252 end time Nov-07-10 05:40:30 PST) it's nice an sharp and leaves an excellent finish.
-Jim
Have you tried a roughing endmill? They're supposed to remove material much more efficiently. I have one but I usually cut stock so close to final size that it's not needed.
I'm also interested to hear opinions on this topic. On my X2 I use 0.02" depth of cut (with 3/8 standard hss endmills) for alu (at the motors' max: 2500RPM) to prevent chatter. Is doing all the work on the tip of the tool a sensible method? I haven't worn one out yet but it's early days!
Hi Jim
I used my cam software to get some figures 1/2" 3 flute EM gave 3800 RPM
The IPM was 7.165 so if you are running at 2000 RPM Then you should be running at 3.5" IPM
But you could run deeper maybe to make up the speed maybe even 1/2 deep in one cut.
I learnt by trial and error as no CNC in my day, hell when i started as an apprentice calculators hadn't been invented, normally you would crank the handwheels by hand so you could feel the cut. Now i have to use feed and speed calculators so i don't get any surprises.
The fact that the machine is shaking is telling you something, i take it you are running cnc as you say you have ballscrews.
Depending on the depth of your slots i would use a drill to rough out slots as drills are very efficient way to remove a lot of metal and are relatively easy to sharpen by hand "With Practice" and save re cutting your chips
What dia is the insert cutter and the amount of teeth ?
As an example 1 1/4" dia 6 teeth is 2700 RPM 39" IPM
If you were making a 3/4 deep slot at .05 DOC you would be making 15 passes and there will be 15 times the amount of wear to the first .05 of the cutter as this is the part that is doing all the work and this will give a noticeable bump at the bottom of the slot as the edge goes off.
I hope this is of some help to you and Alex
Hi Alex thanks for the help. What is the chip load that your CAM software is shooting for? Your example above seems like an exceedingly small chip load. I'd begin to worry about cutter over heating. My cutters stay very cool running at G-Wizards recommend chip loads.
My indexable cutter is 1/2" single flute(insert).
If the machine is shaking, it's telling you you're pushing it too hard. Start with what G-Wiz gives you, with a very shallow DOC. Then go incrementally deeper until the machine starts complaining, or the surface finish starts to degrade. At that point, you're at the machine's limit. Keep the chipload as heavy as possible, to avoid over-heating the tool. If you have to slow the feed, then reduce RPM as well, or the tool will over-heat and clog.
Regards,
Ray L.
Hi Jim, AKA Kingjamez
My name is Phil, as another poster "alex781" was asking similar questions i was answering him as well.
The cad/cam is OneCNC the chipload is .001" per tooth
I suggest you ignore advice for shallow depth of cuts because as i already said shallow cuts mean you wear out the cutter prematurely in a very small area.
The other reason is squaring a billet say 1" thick you want to take that cut at full depth.
The fact that the machine was shaking says Gwiz is wrong or you input incorrect parameters.
Phil
Phil
Hi Phil,
Sorry about that, I saw Alex as the last word in your last post and read that as a signature.
Your 0.001" chipload explains the difference in speed. GWiz suggests a chipload of 0.004" for a standard carbide endmill and 0.007" for an indexable endmill. That's quite a large difference. Perhaps I'll slow down a bit and see how it goes.
-Jim
Hello,
For starters i would recommend getting a Zrn coated Endmill with a variable pitch helix. That should help reduce your chatter and therefore help your machine from vibrating apart. My current favorite is the helical line New Series! | Helical Solutions I run A Haas VF3 so i guess im not really the right person to talk to for small machines but i do know that the right tool makes all the difference. I also wouldn't use a corner radius for aluminum, i do for stainless but i prefer sharp for aluminum, cuts a little nicer i think... My last favorite was the accupro zrn coated, you can pick those up from msc. The helicals i think are about 50 the accupro are a bit more i believe. Ive been running a 1/2 helical at 12000 rpm 180ipm 3/8 doc for a week now and still looks brand new... good luck
Posting Permissions
| | |
