770MX Spindle Keeps Stalling

[shred]

An MX like OP has is a BT30 spindle, but ER20 collet holders are basically the default for that too. I use 1/2" roughers in my 1100MX and they do well especially with a short gauge-length collet holder (Maritool has a nice one), but its a bit bigger machine.

[Joz234]

Question.

What is the max tool diameter in the specs recommended for milling?.

Like shred was saying, my machine is a BT30 taper and I'm using set screw style holders (I own a couple of the Maritime holders btw, so far I'm very happy with them!). I can't find a max tool diameter, but I've found a lot of people using 1/2" endmills happily.
I got some speeds and feeds from some other 770MX users that have the 1/2" version of the tool I'm using, so I'm going to see if I can compare at all. Bob W, the guy that makes GWizard, sent me a couple of emails suggesting that I contact Tormach (I sent him screenshots of my cuts that stalled) as he thinks the machine should be capable. But after reading more people's best practices with the 770MX and similar end mills, I want to try some more testing. I'm just miffed that Tormach gave me such a glowing recommendation for GWizard and sold it to me with my machine. So far it seems to just be the source of all of my trouble...

[popspipes]

I have an 1100 s3 , 1/2" cutters are too large for my machine (chatter) it pulls them OK though so it may just be the type/brand of cutter. I use .25 cutters and down for 90% of my work. 3/8 seems to work well also.

[Joz234]

I have an 1100 s3 , 1/2" cutters are too large for my machine (chatter) it pulls them OK though so it may just be the type/brand of cutter. I use .25 cutters and down for 90% of my work. 3/8 seems to work well also.

I was talking to some people in a Tormach Facebook group that have been using YG-1 1/2" end mills in their 1100MX's and M's with a lot of success, so if you ever feel like trying it again maybe that's the brand to go to! Here are one guys speeds and feeds from an 1100M if you're interested:
10000RPM
.45 DOC
.03 WOC
130 IPM (pushing it a bit)
With this endmill : YG-1: BEST VALUE IN THE WORLD OF CUTTING TOOLS

[Joz234]

Why do so many people get caught in the speed and feed trap?.
It is subjective and depends on a host of factors and conditions.
10 years ago that is all people discussed, argued and hyped day in and day out. Didn't matter if it was big machine or small. Those same people would also talk about how they hand write a g code programs. And how great it all works. I would read this and think what are they making.
At that same time I spent hours modeling parts and then hours in cam software refining tool paths to generate g code. Then focused on material and machine setup to get accurate results with decent finish. The files were often thousands of lines long and require half dozen tool changes. I quickly learned that feed and speeds of tools was only a few parameters in the process and there are hundreds of other parameters that are just as important. Also there was no way your going to do this writing code by hand.

In summary. I focused on drawing and cam tool path skills with good methods for fixturing material and combined those skills with conservative cutter speeds to get drama free results over and over. Then went on to make mountains of accurate shiny stuff and not break a tool. I also learned the faster I tried to make parts the more drama, scrap, tool breaks, and overall problems encountered. But that is the nature of production.
If your learning and making a new widget of some form who cares how fast you do it. Slow is often fast in the cnc machine tool world. And far less expensive.
IMHO your better off getting results first. Then if your making thousands you can refine the many steps to make them faster. Also with experience you learn ways to push your tools and about what you can get away with and not crash machine or scare the dog.

I don't think I did the best job of showing it here, as I didn't post anywhere close to all of the speeds and feeds that I was trying, but at a certain point, I was struggling to get anything to work. I've been told by many people to back things off until they work, which is good advice, but at a certain point, I want to make sure that I got all of the machine that I paid for. I know a lot of people on here run machines much larger than Tormachs, but when I can't make cuts that require more than 0.2HP, and my mmr is <1", I'm surprised most people still thought the issue was the speeds and feeds. In the end, I contacted Tormach and they had me check voltages across the machine, for loose connections/belts, my wall voltage, and they went over my feeds and speeds. They decided that I likely have either a spindle motor with a weak winding or a VFD with programming issues, so they're sending me both parts to swap out.

Overall, it's been interesting to hear everyone's philosophies on speeds and feeds. I think pretty much everyone on this forum recommended backing off my DOC in favor of a deeper WOC, while the folks in the Tormach Facebook group recommended the exact opposite (mainly saying to go for full DOC, and 6-10% WOC, then stepping up the IPM as much as you can. Tormach tech support seemed to side more with this method of cutting, which makes me question GWizard's recommendations even more. Although I've gotta say, Bob from GWizard was the first and pretty much only person to call foul on my machine (other than Tormach). He based his decision solely on the estimated HP of the cuts that my machine was stalling on. This makes me want to go back to leaning on those estimations, but I'm worried it's going to lead me astray...

If horsepower calculations are an inaccurate way of estimating a cut, then this experience has made me wish that the machines shipped with an endmill, a block of 6061, and cad program with Tormachs speeds and feeds to benchmark the machine with! As someone new to machining, trying to figure this out really made me question my sanity (and competence), so someway of benchmarking the machines would be nice for us new folks! Cause God there's a lot to learn!

[mountaindew]

Also, the 3/8" YG-1 end mill (36584) is a 3 flute with a stick out of 2.0556".

This will not solve your hp problem. But for future reference you never want a cutter sticking out 2.0556" unless you have to.
Total indicated runout of a cutter sticking out of tool 2" can be very problematic and chatter on the lightest of cuts. Best to keep tool stick out to minimum. Also your feeds and speeds calculator should have a field for tool stick out or overhang. Enter that 2" number and watch that feed rate drop like a rock.

[Joz234]

This will not solve your hp problem. But for future reference you never want a cutter sticking out 2.0556" unless you have to.
Total indicated runout of a cutter sticking out of tool 2" can be very problematic and chatter on the lightest of cuts. Best to keep tool stick out to minimum. Also your feeds and speeds calculator should have a field for tool stick out or overhang. Enter that 2" number and watch that feed rate drop like a rock.

Thanks for the info! This was definitely an, "I'm new to this" type of problem. I had my tool stick out entered into GWizard and it was telling me my deflection was going to be something like .00066" which it said was "in the green," (and surprising I wasn't seeing any chatter, but I didn't really get a chance to push it to see if I would because of the HP issue). But at Tormach's recommendation, I choked up on it as much as I could to ~1.56" since the flutes are 1.5". I Then switched to using a stub version of the same endmill where my stick out was .52" to make sure that wasn't part of my issue.

This brings me to another question I had. How many sig figs do you normally use when entering, IPM, RPM, etc? I'm guessing with tool length use as many as you can accurately measure, but when I'm getting numbers like 3201 for my RPM or 22.618 for my IPM, do people generally round or keep them all? Thanks for your help!

[dazp1976]

This brings me to another question I had. How many sig figs do you normally use when entering, IPM, RPM, etc? I'm guessing with tool length use as many as you can accurately measure, but when I'm getting numbers like 3201 for my RPM or 22.618 for my IPM, do people generally round or keep them all? Thanks for your help!

The numbers aren't gospel, they're only a guide.
Every machine is different and has it's own limitations.
Until you figure this out and find your own machines limits you'll be in a constant fight of issues.

Lets go extremes.
So GWiz gives you some numbers for a 3/8" end mill, you put them in a haas vmc and it churns out metal. Cool eh?.
Now put the same numbers in a converted hobby mill (like a crap Sieg)... You'll just snap everything, maybe even the column at some point!!!!!.

Now. You are kind of somewhere inbetween the 2.

[kstrauss]

I've never been fussy about entering feed/rpm except when tapping. In your example I would probably enter as 22.6 IPM (or even 22) and 3200 RPM. Besides, I often use the overrides to tweak values based on sound when actually cutting. On older Tormachs the desired RPM is sent to the VFD as an analogue value so it loses accuracy in the conversion. There is little point entering RPM accurately.

[CL_MotoTech]

I've read through this thread a few times and have been kind of hesitant to post because I don't own a Tormach. That said, it sounds to me like there is something wrong with your spindle, spindle motor, belt drive, and you just aren't getting horsepower/torque to your end mill. Your F&S look really conservative. I know it's only a 1.12kw spindle motor, but I bet you have some parasitic drag in there that's costing you HP at the flutes. I had a 1.3kw spindle motor and it would stall quite a lot if I didn't get all the running gear really well setup. With my spindle, if I gave it good hard twist, it would turn a time or two. If it didn't coast, things started to stall despite good feeds and speeds. Every percent counts when you are down on power.

Also, I am a rounder when it comes to RPM and feeds. I don't mind adjusting overrides in process though.

[maker of things]

3/8 diameter cutter is probably on the big side for a 770 in high belt. Have you tried low belt? In high belt you are going to sacrifice torque for rpm. 3/8 is the largest endmill I run on my 1100mx.

Might be worth checking out provencut since the feeds and speeds have been successfully run on tormach. (free trial) If you can't make a cut with one of those recipes then you would have a clear indicator that the motor isn't producing as much as it should.

It's tough getting going and you aren't the first to go have these frustrations and won't be the last, so hang in there.