I am looking at chart calculator from Little Machine Shop.Plugging in #’s at 750 rpm I need 16 IPM so google see that inch’s per minute but what does that mean,what do I seat my feed rate at if it’s range is .0025-.068?I think this is better way to ask question than my other post Better Finish?
-
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!
Speed & Feed?
- Thread starter Kroll
- Start date
I assume you are referring to finding the feed rate on a lathe, right? If so, you are looking for the number of inches per revolution or IPR, which is what your lathe is set up to provide. In your example, you are using 750 rpm and your IPM is 16 inches per minute or IPM so you simply need to divide 16 by 750, or IPM/RPM, and you get 0.021 IPR. Look at the feed chart for a lever/knob setting and set it for the closest one to 0.021 and you should be good.
With that said, charts and numbers and stuff is all fine and good but on a manual lathe you will often need to respond to the cut. Sometimes the speed is too slow or too fast, and sometimes the calculated feed is too slow or too fast. On top of that, feeds and speeds will vary with whether you're roughing or finishing. And on top of that, your tooling will impact on your results; HSS will produce different results vs carbide for the same feeds and speeds so you sort of need to mess with this stuff until you get what you need.
The best idea is to set a depth of cut that is decent, maybe 0.020" deep, and run at your calculated feed and speed and look at the results. Then adjust feed and see what happens, then do the same for speed and so on. Eventually, you will learn what your lathe needs to cut a given material with the tool you're using.
Try not to get married to numbers - your lathe will tell you what it needs if you listen to what it is telling you.
With that said, charts and numbers and stuff is all fine and good but on a manual lathe you will often need to respond to the cut. Sometimes the speed is too slow or too fast, and sometimes the calculated feed is too slow or too fast. On top of that, feeds and speeds will vary with whether you're roughing or finishing. And on top of that, your tooling will impact on your results; HSS will produce different results vs carbide for the same feeds and speeds so you sort of need to mess with this stuff until you get what you need.
The best idea is to set a depth of cut that is decent, maybe 0.020" deep, and run at your calculated feed and speed and look at the results. Then adjust feed and see what happens, then do the same for speed and so on. Eventually, you will learn what your lathe needs to cut a given material with the tool you're using.
Try not to get married to numbers - your lathe will tell you what it needs if you listen to what it is telling you.
Surface speed is another factor. It's simply RPM x pi x diameter. Depending on material, you may want a faster or slower surface speed to obtain efficient removal and a good finish. Surface speed recommendations are found in the same references you find your feeds in. Feed rates and depth of cut mainly are determined by machine power, but surface speeds will arguably play a more important role affecting finish.
Here is what I end up with after playing with speed, feed, and doc. Swarfs fly out like coil springs in 2 inch sections. I am deathly afraid of long strings razor sharp swarf.
FYI, in this situation I could not get the desired outcome without the cutting fluid. There are times I had to cut dry to get the same results
FYI, in this situation I could not get the desired outcome without the cutting fluid. There are times I had to cut dry to get the same results
Last edited:
Thanks guys for responding,just learned that speed/feed apply for lathes drills and mills which I did not know till started looking for chart.Yes it’s a lathe,I am kinda playing around with HSS and carbide inserts but wondering about my grinding and my choice of inserts which is what Shars had suggested.Turning some 1144 stressproof 3/4 rod trying to get that perfect finish.Is there a good chart that you like that I can find and print
Kroll, 1144 is a free machining medium carbon steel with a machinability rating of about 82% (compared to 1212 steel at 100%). LMS lists a cutting speed for HSS at about 70-215 and 670-800 with carbide. You are supposed to calculate your RPM, pick a feed rate and see how that works. LMS's table lists a feed rate of 0.004 ipr when using their cutting speeds so you can start there.
You should know that tables like this can be misleading because they do not take into account what kind of tool you're using. There are MANY kinds of carbide tools and they do not all cut the same. In fact, every insert has their own cutting conditions. Same thing with HSS tools; not all are created equal. I don't know how powerful or rigid your lathe is but that matters, too. I raise this because if you follow the tables blindly then you are likely to run into issues and may not be able to sort out why.
There is no table that takes all of the variables into account. I can tell you what I do and maybe that will give you a place to start so that you can sort out what will work for you.
1144 is one of my favorite materials to work with. It cuts readily and finishes to a nice satin finish. It does not produce a mirror finish with a turning tool, at least not in my hands. Like most medium and high carbon steels, 1144 likes to rough slow and finish fast. I have an Emco Super 11 CD lathe. It is pretty rigid for such a small lathe and it has a 2HP motor that can run at up to 2200 rpm. I typically use HSS with 1144 because it likes sharp tools. For roughing, I use a cutting speed of 40-60 SFM and tend to feed a bit faster at about 0.006ipr. To finish, I speed it way up to 2200 rpm, slow my feed to 0.0018ipr and take very light finishing cuts. This gives me a very fine satin finish.
I also use an SCLCR tool from time to time. I use a CCMT 32.51 and rough at 100 SFM/0.006ipr and finish at my lathe's max speed and I tend to run a slower feed. Depth of cut varies with how much has to come off. Since my insert has a nose radius of 0.015", I tend to rough at about 0.020" depth of cut or more and finish at 0.010 DOC or so.
Your results WILL vary. You have to set your speed and feed someplace and look at your results, then change stuff and see what happens. Sorry but there is no magic formula, no magic table; there is what happens in your shop with your lathe and your tools. I hope you understand that we all have to go through this stuff in order to understand how our lathes cut. It's sort of fun, actually.
Give it a try and don't be afraid to mess up. Play with speeds, feeds, depths of cut, and cutting oils. Eventually, you'll find a combination of these things that works for you.
You should know that tables like this can be misleading because they do not take into account what kind of tool you're using. There are MANY kinds of carbide tools and they do not all cut the same. In fact, every insert has their own cutting conditions. Same thing with HSS tools; not all are created equal. I don't know how powerful or rigid your lathe is but that matters, too. I raise this because if you follow the tables blindly then you are likely to run into issues and may not be able to sort out why.
There is no table that takes all of the variables into account. I can tell you what I do and maybe that will give you a place to start so that you can sort out what will work for you.
1144 is one of my favorite materials to work with. It cuts readily and finishes to a nice satin finish. It does not produce a mirror finish with a turning tool, at least not in my hands. Like most medium and high carbon steels, 1144 likes to rough slow and finish fast. I have an Emco Super 11 CD lathe. It is pretty rigid for such a small lathe and it has a 2HP motor that can run at up to 2200 rpm. I typically use HSS with 1144 because it likes sharp tools. For roughing, I use a cutting speed of 40-60 SFM and tend to feed a bit faster at about 0.006ipr. To finish, I speed it way up to 2200 rpm, slow my feed to 0.0018ipr and take very light finishing cuts. This gives me a very fine satin finish.
I also use an SCLCR tool from time to time. I use a CCMT 32.51 and rough at 100 SFM/0.006ipr and finish at my lathe's max speed and I tend to run a slower feed. Depth of cut varies with how much has to come off. Since my insert has a nose radius of 0.015", I tend to rough at about 0.020" depth of cut or more and finish at 0.010 DOC or so.
Your results WILL vary. You have to set your speed and feed someplace and look at your results, then change stuff and see what happens. Sorry but there is no magic formula, no magic table; there is what happens in your shop with your lathe and your tools. I hope you understand that we all have to go through this stuff in order to understand how our lathes cut. It's sort of fun, actually.
Give it a try and don't be afraid to mess up. Play with speeds, feeds, depths of cut, and cutting oils. Eventually, you'll find a combination of these things that works for you.
I can t nelieve that some of these places that lists speed and feed charts will post up numbers with such a range.
That range for 1144 from 70-215 sfm is quite broad. How is this supposeed to guide someone that is new. In that range your hitting almost all materials from just about Cast Iron to Aluminum with hss.
I hate these charts. What do they do for anyone really. Pick a speed in there a go figure it out doesn t wash with me.
I'd suggest to take a proper look at the materials your using for a more definite sfm.
Here are some sfm for some common materials that make more sense to actually get you in the proper range.
Cast Iron 40-60 sfm, stainless 60sfm, medium carbon steel 80-100, free machining steel 100-140 sfm not including c12l14 which is on par with Aluminum at 200 sfm. This is hss and Carbide will be two to three times as fast.
Add more feed when you have chips like you did to make the chip thicker so it will break vs. roll up.
Different materials will act quite differe here. 1018 for example will chip nice on roughing for me and my lathe from .010-.012" depending on diameter and depth. I may finish at .005" to .007" as 1018'doesn t like to fine of feed vs say 1144 where i may finish at .004". Aluminum I ll rough close to .020" feed rate to break the chip on roughing.
I truly believe the old books and charts are way more reliable and true to materials. They actually knew what they were doing and not putting information out done from computers. Just my opinion but I don t like how machining is taught or done nowadays as they forget the roots and just want answers without knowing how to get there, but I am getting older and half crusty about the machining world today.
That range for 1144 from 70-215 sfm is quite broad. How is this supposeed to guide someone that is new. In that range your hitting almost all materials from just about Cast Iron to Aluminum with hss.
I hate these charts. What do they do for anyone really. Pick a speed in there a go figure it out doesn t wash with me.
I'd suggest to take a proper look at the materials your using for a more definite sfm.
Here are some sfm for some common materials that make more sense to actually get you in the proper range.
Cast Iron 40-60 sfm, stainless 60sfm, medium carbon steel 80-100, free machining steel 100-140 sfm not including c12l14 which is on par with Aluminum at 200 sfm. This is hss and Carbide will be two to three times as fast.
Add more feed when you have chips like you did to make the chip thicker so it will break vs. roll up.
Different materials will act quite differe here. 1018 for example will chip nice on roughing for me and my lathe from .010-.012" depending on diameter and depth. I may finish at .005" to .007" as 1018'doesn t like to fine of feed vs say 1144 where i may finish at .004". Aluminum I ll rough close to .020" feed rate to break the chip on roughing.
I truly believe the old books and charts are way more reliable and true to materials. They actually knew what they were doing and not putting information out done from computers. Just my opinion but I don t like how machining is taught or done nowadays as they forget the roots and just want answers without knowing how to get there, but I am getting older and half crusty about the machining world today.
Guys what is free machining?I’ve seen that in charts but wonder.I have order me book Machinist Ready Reference which was told has lot of info on speeds/feeds.Being a beginner I sneak up on finish OD which finally pass be maybe .002 or so which I am not getting a good smooth finish for a shaft going into bushings.But going go through all these good answers and play around this afternoon
Free machining simply means it tends to form small chips when it is cut, that's all. This allows these materials to run in automated machines without someone having to stand there and pull long stringy chips out of the works.
A poor finish with a 0.002" DOC implies that the tool is not cutting; it is deflecting and skating across the surface. Are you using a carbide tool? If so, what is the nose radius? In addition, many inserts have a radiused edge instead of a sharp one and that makes tiny finishing cuts very difficult to achieve. You can still come in on size but you have to know how to use your insert.
A poor finish with a 0.002" DOC implies that the tool is not cutting; it is deflecting and skating across the surface. Are you using a carbide tool? If so, what is the nose radius? In addition, many inserts have a radiused edge instead of a sharp one and that makes tiny finishing cuts very difficult to achieve. You can still come in on size but you have to know how to use your insert.
"Free machining" is what people think they will get when they bring me a repair to do on my equipment.