X2 Breaking Bits and Horrible Cuts

[webgeek]

Hi all; I feel that I abuse this forum by always asking what seem to be stupid questions but since I'm a noob with no where else to go, I always end up back here. Additionally, this post is a bit of a vent as well as contains a lot of details so it's very long. Sorry about that

Milling on my X2 seems to be getting progressively worse - I really don't know how to describe it better than that. I swapped the gears out for a Steele belt drive and screwed up the spindle in the process so I replaced both it and the pair of bearings. The problems SEEM to have started right around there though I might be totally mistaken. The bearings certainly get much hotter than they used to but that might be due to the increased RPM.

As of right now, I'm using Mach 3 (vs EMC which I used to use and it might also be part of the trouble as it doesn't "feel" like it feeds quite as well as EMC does) and MasterCAM X4. I've gotten pretty good at MasterCAM and finally have it making everything as I'd expect it.

The problem is several fold - I get "screwed up edges" all over the place. This seems to occur near holding tabs the most but sometimes it's just on a flat. I assume this is due to some sort of deflection, I really don't know. This has been happening since the beginning and the deeper the cut the worse it gets.

Also, I've been breaking end mills CONSTANTLY. I've broken four 1/8" HSS end mills today alone. I've basically broken an end mill every other part. This seems to be getting SIGNIFICANTLY worse. To make it more frustrating I've not been able to tell why several of them broke. Usually I've made some stupid and obvious mistake, but these are breaking with no warning and no clear reason why.

Additionally, I now get "rough edges" on all the cuts - basically the swarf is often attached to the lip of the cut. Not sure it's true welding as it's not that severe but it's there none the less. This absolutely started with the upgrade to a belt drive. I'm assuming it has to do with no coolant and the higher RPM but I want to be sure.

Finally, there are occasionally "steps" in the cuts. Flat spots on a curve (does NOT appear to be backlash-style, most like just an odd missed step or something) as well as rough edges on a circle. This seems to have started getting much more noticeable around the switch to MasterCAM but I'm not positive of that either. I'm simply a lot more away of what to expect in general.

I almost always cut 6061 aluminum and I use WD-40 for lubricant and vacuum off the swarf several times per operation. MasterCAM is automatically calculating the speed at ~4 IPM while cutting and a plunge rate of ~2 IPM. The RPM is around ~4300 which is the max my spindle will do. I accidentally had the IPM running at ~6 for a while and to be honest, I broke no more bits than I do now and the cut quality was just as good. That's why it took me so long to notice I had it wrong. MasterCAM was using 4-flute HSS end mills to calculate while I use 2-flute. My depth of cut is always .025" when cutting, facing, or peck drilling. How you guys are able to get a 1/8" end mill to cut 0.125" in a pass is totally amazing to me. I'm breaking them on that 0.025" pass as the picture shown proves.

For clamping, I use a hold down set as well as some flange nuts to pin the piece in place. I used to clamp to wood but when I tightened the material tightly the wood compressed and caused the center of the material being cut to bow up. I now use scrap aluminum as the sacrificial material. Honestly, other than the bowing when I overtightened, I've not noticed any other difference between aluminum vs. wood as a sacrificial material. My end mill holders are all Tormach which I love when I'm not breaking bits and is MISERABLE when I am due to the time it takes to mount and measure a new bit.

As for backlash, I have ~0.003 in the Y axis, ~0.002 in the X axis, and ~0.001 in the Z. I've enabled compensation in both EMC and Mach 3 to address this and measured backlash is now less than 0.001. Some set of the problems has stemmed from things coming loose - the gib screws on the z axis were able to miraculously back themselves out and create a great deal of slop (and wasted parts) before I realized what happened and fixed it.

So after all this, I'm getting the problem is a combination of no flood coolant with higher RPM, possibly missing some steps due to Mach 3 being so damn finicky on some machines (very high end machine and it still doesn't give me nearly as smooth pulses as EMC - not even in the same league) , user error, and ...? I'm just not sure that those things really account for all the problems so that's why I'm here.

I hope this provides enough details for the experts to chime in. I'm pretty desperate here, I was planning on competing at the RoboGames competition in a few weeks but to be honest, I've struggled so much getting parts made that it's highly unlikely at this rate that I'll be ready. I literally planned on months to make the parts and it takes me hours to make a single part good enough. Hell, I bought the Tormach stuff to speed up tool changes - I was that desperate to try and get more productive. In reality, I'm running into MORE problems now than when I first started milling. Low quality, inaccurate cuts, breaking bits - it's enough to make me rip my hair out. My wife is about to make me sell this damn mill just to keep me from driving her up the wall with my own frustration. If someone is interested in buying it, I might be open to the idea to be honest. Any help would be greatly appreciated at this point. Thanks!

-Mike

[wam]

I was having the same problem with my mill what I did was cut the plunge rate to 1 IPM and the problem went away. I am in the middle of a 200 piece job that I am using a 2 flute .09 inch square carbide end mill on t-6061 with a feed rate of 12 IPM. One broke 1 bit at about 190 pieces and the bit was well broken in prior to starting. My problems were cause by my post processor did not take the plunge rate into consideration when cutting bridges. What I did was to write a perl script to re-process the post processed g-code and insert the appropriate plunge rate when necessary. Also, when my plunge rate was too fast and it was causing my Z axis to loose steps. Also, check your gibs for slop...

One other question is how are you bolting your plate to your table. If there is a high spot then your depth of cut will be greater than you expect. I also had this problem. I use MDF as a sacrificial board and swarf was getting under during the milling process. This cause the middle of my 8" plat to bow upward and affect the depth of cut. All I did to solve this was to add another t-nut and screw the middle down.

One other question....what kind of screws are you using.

[hoss2006]

You're stuck with too low rpm for the tool and the SFM is very light for alum. and it shows signs of welding.
Lighten the load with a smaller depth of cut and plenty of coolant.
And air blast as it's cutting with shots of WD will be as good as flood for clearing the chips and keeping it cool.
You don't say where you get your endmills, good stuff will cut like butter, cheap stuff like a butter knife.
Carbide at this size can last longer than HSS.
Hoss

[webgeek]

I was having the same problem with my mill what I did was cut the plunge rate to 1 IPM and the problem went away.

Sorry, which specific problem did this correct?

Also, check your gibs for slop...

That was the cause of the first broken bit of the day - slop in the z-axis of all places. Caused the head to shift when plunging or changing directions on an arc.

One other question is how are you bolting your plate to your table. If there is a high spot then your depth of cut will be greater than you expect. I also had this problem. I use MDF as a sacrificial board and swarf was getting under during the milling process. This cause the middle of my 8" plat to bow upward and affect the depth of cut.

I've definitely had this happen before and I've broken bits because of it. I've gotten pretty good at preventing it by being careful with how I clamp. I also almost always touch off the center of the material, not the edges and then I tell the machine to cut a touch deeper. 0.15" for 0.125" material for instance. This seems to work great and doesn't really have any negatives that I've found. Switching from wood to aluminum as the sacrificial material made a huge difference too and basically eliminated this entirely.

One other question....what kind of screws are you using.

Thompson ballscrews

You're stuck with too low rpm for the tool and the SFM is very light for alum. and it shows signs of welding.
Lighten the load with a smaller depth of cut and plenty of coolant.
And air blast as it's cutting with shots of WD will be as good as flood for clearing the chips and keeping it cool.

Even less than 0.025"? Ugh, parts will take an eternity to cut. Do you guys just use bigger mills typically? Unfortunately I need to use those 1/8" for a lot of my parts. I do use 1/4" occasionally though. And if less than .025, are we talking more like .02 or .015? Sorry, not really sure how much less to go. I have an enclosure that I just finished and it has flood coolant, looks like it's time to move the machine and see how that helps.

You don't say where you get your endmills, good stuff will cut like butter, cheap stuff like a butter knife.
Carbide at this size can last longer than HSS.

I'm using the <$3 end mills from Enco. I know that carbide typically requires more RPM so I'd been shying away from it for that reason. Should I make the jump to carbide? And if so, keep the number of flutes at 2?

Thanks much for all the advice!

-Mike

[hoss2006]

yeah, if you can use a 1/4 endmill for some of the operations, they'll hold up much better.
I'd only use an 1/8 where it's necessary, 1/4 is good for general milling operations.
If you snap a 1/4, you're doing something wrong.
Splurge on a couple good quality endmills ($15+) you'll see a difference.
Hoss

[degreaser]

Take a deep breath, go shoot a target or something. Don't sell the machine.

One thing I'd check is the runout on the new spindle. If it's substantial, it's very easy to break small endmills. Chatter will kill small endmills too. Check the gibs, look for gumming of the endmill.

Just so you know you aren't the only one, here's one of mine. It's a $100 3/4" carbide Accupro that met a chunk of steel at a high velocity. It was on a Bridgeport J series and it stalled the motor. Fortunately it didn't explode. I wasn't happy that day...

[dertsap]

first thing that i see in those pics is cutter deflection
if your using mastercam then use the ramp function and cut the part with a continuous ramp , there is no use in plunging the cutting then profile ,and then rapiding out then plunging again ,
also plunging is never a good idea , especially with a 1/8 end mill

[Teyber12]

man thats discouraging!

Im not sure if a x2 is built anything like an x3 but i had a lot of frustration with slop that turned out not to be in the gibs but the ballnut working loose. Shake the table a little bit if you can fee slop and your gibs are tight try to tighten the ballnut block.

Instead of plunging try ramping as someone mentioned.

I do a lot of profiling on say 1/4" 6061 where i need to do some cutting on the inside that requires a 1/8" endmill. I break a lot of bits as well but nowhere near as big as a problem as you seem to have. I find they break anytime the forces change at all. if there is any slop this will do it. your finish looks like you have a lot of slop. Another thing if if you are clamping this down, when i clamp down anything i notice its easy to get a binding, where the middle of the alu bar is noticably higher then the edges where its being clamped down. If this happens you are going to have a much much higher DOC in the middle then in the edges.

turn on the spindle on a low speed and with a dry rough sponge rub the inside of the spindle. this got all the dirt out of my x3 spindle and lowered the runout from quite high (~.002") to .00025" which is very good.

Maybe posting a video of it cutting would help as well.

Im just trying to think aloud here as i definitely feel your pain and hope to see this problem resolved. If you stick with it think how good you will feel if you solve the problem.

edit: also it looks like you are not taking a finishing pass. I always like to leave .01" or so for the final pass.

cheers

[webgeek]

Don't sell the machine.

Thanks If I sold it, it would be to help pay for a more "newbie friendly" machine that didn't require so much attention and love to produce good results. My friend has a nice little Taig that came CNC ready and he has never really had to address any of these issues I run into - it generally just seems to work for anything he throws at it. I'm not against learning all of these things but I see the CNC machine as a way to make parts - I don't want to be a full machinist, I just want to make small parts with some consistency.

One thing I'd check is the runout on the new spindle.

Both you, Teyber12, and degreaser suggested this as a possible problem. My understanding was that the Tormach TTS used the face of the spindle vs the inside like a typical collet. So the runout would need to be the physical spindle in the bearings vs a collet in the spindle. With that said, I'll go back and do as you suggest and try and smooth it down a bit.

if your using mastercam then use the ramp function and cut the part with a continuous ramp, there is no use in plunging the cutting then profile ,and then rapiding out then plunging again

Ok, so is this the "Contour Type" setting of "Ramp"? It disables my use of depth cuts so I assume I'd set the "ramp depth" to the same value as the "depth cuts -> max rough step" that I'd previously been using? I hope the setting you are refering to is something else though as this setting also disables holding tabs which are critical to my parts. As for plunging, it never made sense to me either but I never saw a clean solution to it. I'd been using entry and exit paths just so I didn't plunge right next to the part. This helped a bit, but not nearly as much as I'd have liked.

if there is any slop this will do it. your finish looks like you have a lot of slop.

The table and gibs "feel" tight. There is no slop that I can feel in any axis. I used to have a lot of slop and it caused visible backlash issues but tightening everything down seemed to fix it. I'll double check again to be sure.

Thanks for all the advice and such, I'm going to go give a lot of it a shot right now!

-Mike

[knudsen]

Cutting slots it tough on a little mill. I find it works better to go with a shallower cut, higher RPMs and feed it faster. I turn handles though, so I can feel it before it breaks (sometimes )

[BobWarfield]

Lots of good advice here.

The first thing I'd emphasize is the need to clear chips, especially when slotting. If you see chips building up at all when cutting a full width slot, you aren't doing enough to clear them. Get a continuous air blast going that's aimed at the cutter. Easy to rig up and you don't have to run that much pressure to keep the chips clear.

I would have thought you could run a 25 thousandths depth slot with your 1/8cutter, but maybe not. Keep a notebook of what works and what doesn't as you learn what your machine is capable of and try lots of experiments. For example, maybe you can only cut 15 or 20 thou on the full width slot, but once you have a slot all the way around the profile or pocket and you get ready to hog out more you could go deeper.

In terms of cutters, two thoughts. First, if you want more rpm but don't have it, try a 3 flute instead of a 2 flute. They're like having a 50% faster spindle. I like Maritools 3 flutes. Second, the 1/4" was mentioned, but I really like a 3/16". I'd get 2 or 3 of the 3 flute endmills in 1/8, 3/16, and 1/4 and always use the biggest one that will fit.

FWIW, try a little faster feed too. G-Wizard suggests 10 IPM for a full slot, 4300 rpm in 6061 with a 1/8". Sometimes moving too slow makes little chips that get coated with coolant (especially WD-40) and are more likely to weld it seems like. I find this moreso with cast tooling plate than 6061, but its worth a try.

Lastly, maybe there is some toolpath issue. I was having a terrible time on one part and finally figured out that at one certain point my CAM program had created some g-code that rapided down into the part. It thought it had clearance, but it was catching just a little and was chipping the endmill.

Best,

BW

[webgeek]

Thanks everyone for all the great advice. Here is what I tried this evening:

1) Slow down all plunges to 1 IPM
2) Use my flood coolant system/enclosure - it leaks like a sieve but does spray coolant everywhere
3) Change the depth of cut to .015

I think the end result speaks for itself. The attached photo is of the same part as before but with the new setup. I took it right off the mill and it looks as you see it. I still get a tiny bit of screw up where the holding tabs are but it's less then before and really tiny this time around. Sadly, the part took FOREVER to make but the nice thing about CNC is it's "fire and forget" nature so I'll just walk away and let the machine take it's sweet time doing it right.

Thanks again for all the help on this!

-Mike