The snip you quoted removed important context. You are correct in the technical sense. Electrical power cannot be increased. The power delivered; i.e., torque, can definitely be multiplied by gearing. The net result is the same; the workpiece has more force turning it.
-
Welcome back Guest! Did you know you can mentor other members here at H-M? If not, please check out our Relaunch of Hobby Machinist Mentoring Program!
What's a decent cut for a 9x20 import?
- Thread starter durableoreo
- Start date
One of my criteria for DOC wouldn't fly in a commercial shop. If the chips are flying very far, as onto me and very many of them going to the floor, I reduce the DOC. I can afford to take a little longer to get to the desired OD since all of my work is donated as a volunteer anyway.
- Joined
- Sep 10, 2022
- Messages
- 1,131
Funny little story. The place I am at now the people take slow light passes. I had a chunk of CRS that was 8” dia. I had to turn one se toon down to 4”. I was taking .200 /side passes with coolant. They started complaining about all the smoke and chips flying. I was told to dial it back.
Cutting oil is my blood.
- Joined
- May 3, 2020
- Messages
- 369
He uses a depth of cut of 0.5 mm, which is about 0.020" The feed is heavy, which is apparently what you should try first.
(I'm not buying the first half, in which he claims to take 1 micron passes. Gotta see the micrometer to believe that.)
- Joined
- May 3, 2020
- Messages
- 369
OK, thanks, that's inspiring. I've been pushing here and there. I had a bunch of good cuts at 0.040 and some at 0.050. At some point I had some trouble with a chipped insert, which resulted in a lot of chatter. Then the replacement insert chipped on the first pass but I didn't notice. Took a while to figure out if it was the depth of cut, insert, or just the diameter I happened to be cutting at the time. Chips are silver when cutting near the center (0.625) but fairly colored as I approach 2.280".
Since then, I've started hand-sharpening the inserts. They're CCMT-060204 which is just a little guy. I've been touching them up on a cheap metal-bond diamond stone. They hold up fairly well, maybe better than factory for heavy cuts. It's not exactly the same as off-hand grinding HSS tools but it's not completely different, either.
I'll push toward 0.050 again tomorrow, with freshly honed inserts.
Thank you for the complement.
- Joined
- May 3, 2020
- Messages
- 369
I don't know why I responded like you're not right here. No offense intended. Thanks for adding to the performance conversation. You and @RaisedByWolves get the prize for video documentation of claims.
Regarding your video, when cutting steel, depth of cut is 0.020 in and feed is 0.005 in/rev. That's 0.30 cubic inches per min, if I calculated correctly. Not too shabby for a mini lathe.
For comparison, I was getting 0.4 cu in / min with a depth of cut of 0.030 in, 0.005 in/rev, and 600 RPM (average).
Here's the schedule for the bore, which starts 0.625" and is enlarged to 2.2. It's 28 passes at 0.030. Stepping up to 0.035, which feels like nothing when standing at the machine, brings it down to 24 passes. That's a savings of about 3 min per part. A cut of 0.040 brings the total to 21 passes, which saves 5 min per part. I'm doing another batch of 15 parts, so this saves 75 min.
Stock MMR
Pass diameter in^3/min
-------------------------
1 0.625 0.177
2 0.685 0.194
3 0.745 0.211
4 0.805 0.228
5 0.865 0.245
6 0.925 0.262
7 0.985 0.279
8 1.045 0.295
9 1.105 0.312
10 1.165 0.329
11 1.225 0.346
12 1.285 0.363
13 1.345 0.380
14 1.405 0.397
15 1.465 0.414
16 1.525 0.431
17 1.585 0.448
18 1.645 0.465
19 1.705 0.482
20 1.765 0.499
21 1.825 0.516
22 1.885 0.533
23 1.945 0.550
24 2.005 0.567
25 2.065 0.584
26 2.125 0.601
27 2.185 0.618
28 2.245 0.635
-------------------------
mean: 0.406
There's about 3.1 in^3 of material to remove, which should take 7-8 min if I was cutting continuously. Retraction, setting up the next cut, and maintaining the tool all add up to more than half the time spent on each part.
Last edited:
I am not offended in any way. There are more people that find it hard to believe that a Chinese mini lathe can cut repeatedly at such a small depth. I think is has more to to with the lack of ball bearings in the X-axes, the very modest acceleration to prevent overshoot, retracting at least 0.25 mm (0.01") to get some movement in the X-axis and doing it CNC controlled. I can't do it manually.
I you do the math (a dutch cnc zone member did it for me), you will find that for 0.001 mm depth of cut with a 0.4 mm tool nose radius, the feed should be max 0.04 mm / rev otherwise cuts will not overlap. So I was running to fast. I repeated the test at 70% overlap and it still cut.
But even if it cut's every pass, it doesn't mean it cuts every pass 0.001 mm so it is surely not that accurate.
To get this resolution I had to increase the micro stepping (from 4 to 8 micro steps). That is doable for testing, but not for real life turning. Besides that, it makes no sense having a resolution way higher than the accuracy that can be achieved. I
I normally never "stress" my mini lathe doing 0.5 mm cuts on steel. Even on my bigger lathe I rarely do this. Not because they can't handle the load but because the chips get every where in my very small hobby shop.
Guys, the definition of power is "work performed over time." Watts are joules per second, for example. Torque, on the other hand, is force applied at a distance from the center of a rotating mass, as in pounds-feet or inch-pounds, without reference to time. Torque can be entirely static, as when we are just finished tightening a bolt. Gearing increases torque, but slows down the rotation, so the force is higher but the speed is lower, resulting in the same power.
Torque is what pushes a tool through a material on a lathe, but power is what dictates how fast we can do that pushing. A given volume of material removal will take the same power (assuming constant efficiency, which is an unrealistic assumption that would also have to take tool geometry and material into account) whether or not we use a shallow depth of cut at high speed or a deep cut at low speed.
Lathes that slow the speed electrically rather than using gearing will not see the torque multiplication because the motor itself will produce less power when slowed down that way. That undermines the reciprocal relationship (again, assuming constant efficiency) between force and time.
I had learned this in physics, but it really came home to me when comparing engine torque and power ratings. Many high-power engines have to turn 8000 RPM to get that high power, while many high-torque engines have low horsepower rating simply because they can't turn fast enough to generate high power ratings. A diesel truck engine may produce a 1000 ft-pounds of torque but may do it at 1200 RPM and red-line at 2000 RPM. H=T x RPM/5252, so that engine will produce 380 HP at 2000 RPM. A car engine that produces 380 HP at 6000 RPM may only produce 330 ft-lbs of torque at some much lower RPM, maybe in the 3000-3600 range. Both will take the same amount of time to do the same amount of work. (Again, assuming constant efficiency, plus trucks are, of course, much heavier than cars, so "the same amount of work" takes some effort to imagine.)
The notion of speeds and feeds are a consideration of the efficiency of the tool and material combination. The charts suggest what speeds and feeds will produce the highest tool-cutting efficiency, but that may not be the highest efficiency of the lathe. Those charts assume the lathe has abundant power to handle the suggested speeds and feeds.
Rick "Archimedes" Denney
Similar threads
