Now you are at the point where you have your lathe hooked up to power, and tested all the movement, and you have it leveled.
What’s next??? Tooling of course!!
My first concern was regular profile turning tools. I really didn’t want to spend a fortune on tools, and when you get to tooling for a machine of this size, individual holders can really creep up in expense. Luckily, there are a lot of options out there to do this and still be conscious of your budget. My largest holder was a 1/2″ that I used with my old Southbend Magnaturn 612, but I didn’t want to do that much shimming to use those in my new lathe.
The best solution I’ve found, and purchased for each of my lathes, is a full set of holders in a nice box with all the tools, and inserts. The inserts are adequate, but are great while learning so you aren’t destroying expensive inserts.
Both of these sets are available from Shars.
The inserts are not necessarily the best, but,
the holders themselves are fantastic.
I personally ordered the set shown on the left. The Automate lathes are actually designed for a 20mm insert, so you will have to shim them a little bit. I’ve found that 0.030″ shim pretty much gets them right on center without any problems.
The set on the right is a new offering that I recently found which has boring bars too. I have used some of Shars boring bars, but not this specific set. In my experience, I have found their boring bars to be very nice quality as well.
Since I just mentioned boring bars, this might be a good time to discuss a bit about tooling your lathe up for boring bars. The turret I have on my machine has 8 positions. 5 are for profile type tools, and 3 are for boring/drilling type tools. However, I was a BIT lost at first as the holes in the turret for boring were 1.25″ dia openings. I had no clue what I needed to do as far as mounting to be able to use them.
My first thought was getting some ER type collets that had a 1.25″ shank. Yeah, that wasn’t going to happen as those are seriously expensive.
After some discussions and talking with other folks with bigger lathes, I found out about resizing bushings.
Bushings from Amazon
These bushings I got off Amazon. I ordered 3 of them so I had 1 for each of the boring tool slots on my turret. Then, I also purchased some ER-20 holders with a short 3/4″ diameter shank. I could have bought the bushings in different sizes, but the ER-20 collet holders make it so nice, as you only need to choose a collet to match the size of the shank of the tool you want to use, and you are done.
ER-25 Holders from Amazon
For the gang tool holders, they had 1″ diameter holes, so I bought some ER-25 holders to use on the gang block.
Awesome, now you have tools, how do you set them up?
I’m sure there are different methods, but the simplest I’ve found is to reference the tool off the face of your chuck. It’s a known point, and easy to get back to. There is one disadvantage, and that is if you change chucks. I normally use a collet chuck, but, when I have to switch to my 3 jaw chuck, I do have to reset the Z. Not a huge deal, but it is something to realize. I do try and setup my tooling prior to mounting the 3 jaw chuck, but if I bump something or nudge something I’m pretty much resetting all of my Z offset for all of my tools
I use a magnetic tool setter for this purpose. I lay a parallel across the 2 little nubs on either side of the large button on top, and adjust the dial to Zero. Then I use the mag base and stick it on my chuck. Then for each tool, you move in SLOWLY until the needle shows zero, at which point, you set your Z offset to 2.000, as that is the height of the zero setter. This means that the FACE of the chuck will wind up being Z0. One thing to note, I never try to get too close to that Z. Most of my cuttoffs occur at the Z1.000 mark.
Setting the X axis is a little more odd, but really, all you have to do is turn on your spindle, and use the jog pendant to make a cut on a piece of scrap material. Make sure you are doing it nice and slow so you have a smooth clean cut. Once you have made a cut , jog back away from the material in Z only. Then use a caliper or a micrometer, and measure the diameter of your cut. Go back into the control, and enter in your X offset which is that diameter you just measured.
Well, for most tools, yes, but ultimately, not always easy. Some tools are quite easy, but when you get into tools that have a cutting edge in different areas of the tool holder, it can get a bit tricky.
For example, the tool picture below can be a little difficult to get the point setup properly.
In the case of the this particular tool, I measure the distance from the side of the tool facing the chuck. In the image above, it measure 0.367″. Remember that number. Now, touch off the side of the tool marked with the red arrow, and do the Z offset at 2″, just like you would on a tool with a leading cutting point.
Here’s my solution for this.
We setup the tool at 2″ because that is the height of the Z offset of the indicator I am using.
Now, if you do the math:
2.000″ – 0.367″ you get 1.633″.
Now, just jog the Z for that tool to 1.633″ using your pendant, and reset the offset to 2.000. Now, the point of that tool is at exactly 2″.
I setup all of my tools that don’t have a leading cutting point by using the same method, even a knurling tool.
Speaking of knurling tools…
Since we now know how to setup these kind of tools for Z, how do we do a knurling tools offset for X?
This is the knurling tool I typically use. As you can see, it’s been well used!
This tool is actually a 1/2″ sized tool, so I have to use some slightly large spacers
in my Automate FL300-II lathe, but it still works!
You have already setup some cutting tools X offset by doing test cuts on some scrap material. Just measure the diameter of the last cut you did, and jog the knurling tool toward the scrap material on X until it starts to spin. There’s your X offset for a knurling tool!
I would suggest you use a slower RPM for setups, 500-1000 is my suggestion.
Setup of the Inner Diameter or Boring tools…
Setting up the boring tool on Z is going to be done the same way as previous described, using the Z offset indicator.
However, X is a little bit different. The main thing to remember for setting up X is that you need a hollow in your scrap stock. Go ahead and drill that out, and then use the jog pendant to move in and do a nice slow ID cut in Z, and back it out again, giving a nice smooth finish.
Now, using the measuring device of your choice, measure the ID of the hole, and enter that number into your X offset on the control.
And the last one i’m going to mention today is drills….
Putting it simply, after learning about this tool from a good friend, I realized I had been centering holes on lathe and mill in a much more difficult way than I needed to. This device has become one of my trusted shop tools, and I always have a spare on hand now. You can find these on ebay fairly reasonably.
They come with a bar that you screw into the indicator. Then you mount the indicator in the spindle of your lathe, and put in an appropriate length tip (the kit comes with quite a few). Then you jog the X & Z until the “tip” is inside the boring tool slots in the turret. At this point, turn on the spindle at a low speed, something like maybe 100-200 rpms. Now, all you have to do is jog the X in .0001″ increments until the needle stops jumping. That tells you that your spindle is now centered to the location on the turret. Simply enter 0 into the X offset on the control, and your drill bits will be nicely centered!
NOTE: You can use this same tool on your mill for centering on holes if you’re doing 2nd op machining.
One last thing I will mention is that my new Automate Lathe and even my old Southbend Magnaturn 612 both have repeatable reference points. With some lathes out there, the reference switches are not quite repeatable enough, so you have to calibrate those manually. Z calibration is typically done by a touch-off on an indicator, and X is calibrated by making a test cut on scrap, measuring that test cut, then you use that value for setting the X reference.
Well, that’s probably enough for this article. I hope the information helps you out there.
Thanks for reading, and keep an eye out for my next article where I talk about the first cuts with my machine.
Mandala Rose Works, LLC
Check out more videos here.
For more on tooling up your lathe, check out the article on how I set up the turret on my cnc lathe.
Wade Wendorf runs and owns a company called Mandala Rose Works, LLC which for the last 8 years has designed, manufactured and produced a unique machine called a Rose Engine Lathe targeted at the home woodworker and hobbyist. In addition to building and selling his Rose Engines, he also does prototyping and short production runs of parts for various customers.
Like what you read on CNCCookbook?
Join 100,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Just enter your name and email address below:
100% Privacy: We will never Spam you!
Hi this is Joseph S Romano I need some experience on CNC citizen Swiss with a LB12 Bar Feeder.
I’m open to suggestions at this point.
What exactly are you looking to do with the barfeeder? Is it a cav barfeeder? I just purchased a Citizen L-12 with the cav barfeeder so I’ll try and help you
Sorry Joe I just realized it’s an lb-12 I didn’t read your post correctly.
My lathe doesn’t have limit switches for home, I’m told it homes using a “floating zero”. Do you have any articles on how to do this, I’m a bit lost at what is the best way.
I made an update the the article today that talks about how to do that if you don’t have reference limits.
Here is my comment on that, quoted from the article:
“One last thing I will mention is that my new Automate Lathe and even my old Southbend Magnaturn 612 both have repeatable reference points. With some lathes out there, the reference switches are not quite repeatable enough, so you have to calibrate those manually. Z calibration is typically done by a touch-off on an indicator, and X is calibrated by making a test cut on scrap, measuring that test cut, then you use that value for setting the X reference.”