[ZeroBacklash]

I recently purchased a used Emco Unimat lathe. Model no. is not mentioned on the name plate. I gather it would be a DB200 or SL1000 or even an older machine than that.

Attachment 393880

I am planning to retrofit this to a CNC.
Currently I have planned for 4 motors

1. Replace Universal spindle motor (this seems to be around 100W) to a 100-150W BLDC motor with speed control.
2. Stepper Motor (7kg-cm, NEMA17) for tool X movement.
3. Stepper Motor (7kg-cm, NEMA17) for tool Y movement.
4. Stepper Motor (10kg-cm, NEMA17) for tailstock linear movement) for drilling and threading operations.

Will Mach3 or any other software will be capable of controlling these 4 motors. I mean does any CNC software support speed control of spindle motor and also tail stock motor control for drilling tapping. In this case what kind of controller will I need for the spindle?
I am aware that x and y axis need a driver that will receive step / direction signals from Mach3 but am not so sure about Mach 3's capabililty at handling 4 motors.

If Mach3 cannot do this is there any other software that can achieve these functions?

Thanks in Advance.

[JohnHaine]

Mach 3 will certainly manage a 2-axis lathe and control the speed of the spindle, and with a suitable spindle sensor will do threading. Lathes don't normally do cnc drilling from the tailstock, the drill would be mounted in a suitable holder on the carriage possibly with automatic tool changing. In mill config Mach 3 can control 3 axes plus spindle, but not in the standard lathe config.

[ZeroBacklash]

Mach 3 will certainly manage a 2-axis lathe and control the speed of the spindle, and with a suitable spindle sensor will do threading. Lathes don't normally do cnc drilling from the tailstock, the drill would be mounted in a suitable holder on the carriage possibly with automatic tool changing. In mill config Mach 3 can control 3 axes plus spindle, but not in the standard lathe config.

Thanks for your valuable inputs.
From your post I believe I can at least achieve spindle speed control, and x, y control of tool carriage with Mach 3 right? And I also would need an encoder for the spindle?.
I just need to check on suitable spindle motors.
With regard to the tail stock in threading mode, the tapping tool is mounted into the tailstock right? so wouldn't that need to be controlled in a reciprocating motion for proper thread profile?

Also is it necessary to add some anit-backlash for the cross-slide ?

[JohnHaine]

"From your post I believe I can at least achieve spindle speed control, and x, y control of tool carriage with Mach 3 right?"

Correct.

"And I also would need an encoder for the spindle?"

Yes if you want to do threading and have Mach 3 control spindle speed. Mach 3 can only cope with a single index pulse per rev which it uses to synchronise threading. However, though threading works OK for me with a Myford Super 7 with plenty of power and inertia in the chuck, threading sync may not work so well on the Unimat unless you take the lightest of cuts. The encoder can be a slotted disc on the spindle with an opto-interrupter.

"With regard to the tail stock in threading mode, the tapping tool is mounted into the tailstock right? so wouldn't that need to be controlled in a reciprocating motion for proper thread profile?"

No! You can thread from the tailstock using a tap but it's essentially a one-pass operation - you know what a thread tap is I assume?

In the lathe, external and internal threads are cut with a single-point tool on the carriage, which is moved in sync with the spindle to form the thread. On a normal lathe this uses gears; in CNC the sync is done by the controller. For internal threads the tool looks like a boring tool but has a pointed tip to match the thread form. For external threads again you have a pointed tool. Typically you might be cutting a 1mm deep thread in 10 x 0.1 mm passes, or even more passes with less infeed.

For a lathe, it is useful if the cross slide has minimal backlash - I have fitted a ballscrew to the S7 x-slide. It isn't so important in the Z direction because you are almost always cutting towards the chuck, so I use the standard leadscrew. I doubt you could fit a ballscrew on the Unimat so you could experiment with a Delrin nut or a split nut.

From your questions, I suggest that you download the Mach 3 turn manual and read it carefully, especially the part about threading; and also a book on ordinary non-CNC lathe work.

[ZeroBacklash]

Many thanks again these are amazing insights and it has certainly been a highly enlightening experience reading your posts!

[ninefinger]

For control software there is also LinuxCNC - LinuxCNC
Index of /testing-stretch-rtpreempt this is the best place to get it currently - includes the operating system. Totally free if that matters...
Can run through the parallel port (Mach3 compatible type BOBs) or other control cards (Mesa plug in pcie cards or ethernet cards, and others .
Although there is initially a bit more learning involved, the LinuxCNC software is very adaptable and great to learn on as its scaleable to larger and more complicated machines, plus doesn't have the quirks that Mach 3 is known for (and isn't dependent on a 16 year old operating system).

For threading LinuxCNC can take in both the index pulse and an encoder pulse for better control while threading ( with the caveat of more inputs and need for more configuration).

I've got it in use on a lathe and a mill - and I've used it with standard parallel ports and the mentioned Mesa Ethernet cards and I think its great.
Cheers,

Mike

[ZeroBacklash]

For control software there is also LinuxCNC - LinuxCNC
Index of /testing-stretch-rtpreempt this is the best place to get it currently - includes the operating system. Totally free if that matters...
Can run through the parallel port (Mach3 compatible type BOBs) or other control cards (Mesa plug in pcie cards or ethernet cards, and others .
Although there is initially a bit more learning involved, the LinuxCNC software is very adaptable and great to learn on as its scaleable to larger and more complicated machines, plus doesn't have the quirks that Mach 3 is known for (and isn't dependent on a 16 year old operating system).

For threading LinuxCNC can take in both the index pulse and an encoder pulse for better control while threading ( with the caveat of more inputs and need for more configuration).

I've got it in use on a lathe and a mill - and I've used it with standard parallel ports and the mentioned Mesa Ethernet cards and I think its great.
Cheers,

Mike

Thanks for sharing your wonderful experience.
I wish I had reach you post earlier currently for the emco unimat I have purchased

Nema 17 stepper motors 4kg-cm bipolar for the carriage
Leadshine DM422 stepper drives
For spindle I am thinking of Leadshine DC brushed servo 80W, 3400RPM, DCM50205
And for the servo drive Leadshine DCS303
For the motion controller UC400ETH from CNC drive
For breakout board HDBB2 from CNC drive.
Software I am planning UCCNC from CNC drive

I wasn't aware that you go do without the motion controller(I was planning to run this system on Windows), because I had read a lot of posts saying that a PC might not handle so many realtime motion of 2 x, y and also spindle motor, I had even planned to motorize the tail stock.

[ZeroBacklash]

@hfjbuis

I have seen you build at the link you earlier posted.
1. Did you do any backlash elimination for leadscrews of the z-axis (carriage) and x-axis (cross slide). Are there any general guidelines to eliminate backlash via hardware / software?
2. What kind of accuracies do you get for this build?
3. What feed rates do you generally run at for say mild steel?
4. Are geared stepper motors preffered to non-geared ones?

[hfjbuis]

1. Did you do any backlash elimination for leadscrews of the z-axis (carriage) and x-axis (cross slide). Are there any general guidelines to eliminate backlash via hardware / software?

I implemented backlash compensation (elimination) in (my) software (X,Z and C-axis). It could be done in hardware, but that would mean a change in the controller software (GRBL). The GRBL developers decided that this feature could and should be resolved in the CAM or GUI software. I agree to this.
Basically you have to compensate for backlash at every change of direction. This could be done in hardware. But when i chamfer during threading and move from the Z- to the Z+ direction (to the start of the thread) and then would chamfer by moving the threading tool in the X- direction, the carriage would / could move in the Z+ direction by the force of the tool. So before the chamfer X move, i move the carriage 0.001 mm in the Z- direction. There is no way, the hardware could do this so it can only be done in the CAM or GUI software.

2. What kind of accuracies do you get for this build?

Accuracy depends on the play / setup of your machine and of course the wear. I modified the sliders for the carriage that made my mini lathe more rigid with less than 0.005 mm play. You should do this anyway. At the moment I am redesigning these sliders and will replace them with a ball bearing.
After the setup, I tighten the top slide gib screws.

In general i can turn the diameter accurate to 0.04 mm without measuring or adjusting anything independent of witch of the 10 turning tools I select.
When I measure the diameter before the last 0.1 mm to turn, i can turn withing 0.01 mm. If i don't change the tool, i do not need to measure again.
I did a test on how thin i could turn aluminum using a CCGT060204 insert. Even when turning 0.001 mm down each time, I still could see it was turning, not rubbing and it was turning each of the 10 passes i made. Needed a magnifying glass to see this! This was impressing and means that the positioning of the X-axis is repeatably very good.
The accuracy of positioning the Z-axis is also repeatably very good. I can't measure this but when i repeatedly face 0.01 mm off, it is facing each pass. So the positioning of the Z-axis must be within 0.01 mm.
I checked the positioning of the Z-axis using a iGaging DRO. Over a total length of 200 mm, the values from the iGaging DRO differs no more than 0.02 mm from the CNC DRO.
Beware

• These measurements are done with very little stress on the machine so there is very low influence of the rigidity of the lathe.
• The measurements are done, moving the axis in the same direction.

Backlash compensation is a bit complex on my lathe. There is a difference of 0.04 mm between the first and the second pass in the same direction on the Z-axis. I think this is caused by the modified sliders under the carriage. That is why I am going to change them for a ball bearing type. Then I expect more accuracy but less rigidity.

3. What feed rates do you generally run at for say mild steel?

I usually turn small parts and run slow between 30 and 60 mm/min and 100/500 rpm. I could run faster, especially when using insert tools, but it would give more stress on the machine (more wear) and less accurate turning because of the deflection of the part. I only make prototypes and time is never an issue.

4. Are geared stepper motors preferred to non-geared ones?

My X-axis is driven directly by a Nema17 0.5 Nm stepper.
The Z-axis is driven by a Nema17 0.5 Nm stepper, geared down 20/60. I needed more torque and the gearing covered the distance between the stepper and the Z-axis.
The C-axis is driven by an Nema24 4Nm stepper, geared down 20/45. If I would do it again, i would gear it down 20/100 just for threading large diameter (60 mm) Cr42Mo4 steel. I never run this C-axis at it's max speed!

I used the original plastic (POM) lathe gears. I made some of aluminum but they made more noise than the plastic once so i switched back to the plastic once. Until now, i didn't wear out a gear nor broke one. This is one of the advantages of using low torque steppers and not running at high speeds.
Geared steppers a very compact and expensive but also longer. Once you buy them, you "can't" change the gears. So for the first machine (prototype), I would go for external gears.

[ZeroBacklash]

@hfjbuis, Thats a thought provoking extended reply. Many Thanks!

ok so by sliders you mean the long screws that run either of the axis right?
i have posed this question for a bigger lathe machine, I will post pics soon. The bed of this lathe as around 4 feet long, Z axis lead screw could be 6 feet long and x-axis screw may be around a foot long.
I have not done any tests for play/ backlash on this machine. But considering its a used machine I have a feeling that there would be considerable play.

So do you do backlash compensation in your software, CNCL? is this just a number to be fed into the software, and once set will the software do the necessary corrections like retracting the axis a particular amount before any direction change? I would feel that you would need to move the axis a few microns ahead due to the play in the thread interactions instead of retracting them, this way the threads will mate during the initial baclash compensating movement and then would start the actual movement for machining.

I am considering using 7Nm geared stepper for the Z axis and 4Nm for the X axis, right now these 2 axis are all I need, I will add the spindle (C-axis later).

[skrubol]

I recently purchased a used Emco Unimat lathe. Model no. is not mentioned on the name plate. I gather it would be a DB200 or SL1000 or even an older machine than that.

Attachment 393880

I am planning to retrofit this to a CNC.
Currently I have planned for 4 motors

1. Replace Universal spindle motor (this seems to be around 100W) to a 100-150W BLDC motor with speed control.
2. Stepper Motor (7kg-cm, NEMA17) for tool X movement.
3. Stepper Motor (7kg-cm, NEMA17) for tool Y movement.
4. Stepper Motor (10kg-cm, NEMA17) for tailstock linear movement) for drilling and threading operations.

Will Mach3 or any other software will be capable of controlling these 4 motors. I mean does any CNC software support speed control of spindle motor and also tail stock motor control for drilling tapping. In this case what kind of controller will I need for the spindle?
I am aware that x and y axis need a driver that will receive step / direction signals from Mach3 but am not so sure about Mach 3's capabililty at handling 4 motors.

If Mach3 cannot do this is there any other software that can achieve these functions?

Thanks in Advance.

What kind of BLDC motor are you planning on using? If you're thinking an RC motor and speed control you may have some issues. Generally 3-phase induction motors are used with VFD's, but finding fractional HP setups at prices you would be happy with might be an issue.

I'd skip the tailstock stepper and leave that manual. Drilling and tapping one-offs don't usually need CNC that badly, and if you have something you do want to automate, put the drill in a toolholder. What are you planning for a tool post? At the very least you'll need a decent quick change toolpost.
Are you planning on using the existing screws?

[ZeroBacklash]

What kind of BLDC motor are you planning on using? If you're thinking an RC motor and speed control you may have some issues. Generally 3-phase induction motors are used with VFD's, but finding fractional HP setups at prices you would be happy with might be an issue.

I'd skip the tailstock stepper and leave that manual. Drilling and tapping one-offs don't usually need CNC that badly, and if you have something you do want to automate, put the drill in a toolholder. What are you planning for a tool post? At the very least you'll need a decent quick change toolpost.
Are you planning on using the existing screws?

I was intially planning on a BLDC BLM57090 from Leadshine but currently I am settling on a DC brushed servo model no. DCM50205 its a 80W, 3400RPM, peak torque seems to be 3Nm.
Here is the link
Leadshine Brushed DC Servos

Now when I see the drive specs DCS303 it shows only step and dir inputs and not 0 to 10V so I was thinking is this the right motor for this application.

[hfjbuis]

I do threading using a stepper (Nema23 2Nm) mounted on the spindle and control it as C-axis. This works fine and you can do any pitch threading. No need to have a box full of taps. For most jobs, 2 Nm is strong enough, can't even run it at max speed otherwise deflection of the part will be to much. And for the larger threads, just reduce speed and cutting depth. Takes i bit longer but who cares, it runs automatically. I recently changed to Nema24 4Nm because i had trouble threading ER32 (M40) on Cr42Mo4 steel. Works even better though i found out today the problems where caused by the power supply (now outputs only 14 Volts). If you have a stepper mounted on the spindle, you can do other cool things like broaching, knurling and grinding drills and end mills. It turns your lathe in a very versatile tool.

[ZeroBacklash]

I do threading using a stepper (Nema23 2Nm) mounted on the spindle and control it as C-axis. This works fine and you can do any pitch threading. No need to have a box full of taps. For most jobs, 2 Nm is strong enough, can't even run it at max speed otherwise deflection of the part will be to much. And for the larger threads, just reduce speed and cutting depth. Takes i bit longer but who cares, it runs automaticaly. I recently changed to Nema24 4Nm because i had trouble threading ER32 (M40) on Cr42Mo4 steel. Works even better though i found out today the problems where caused by the power supply (now outputs only 14 Volts). If you have a stepper mountedon the spindle, you can do other cool things like broaching, knurling and grinding drills and end mills. It turns your lathe in a very versatile tool.

That's amazing to hear I intended to do that (mounting a stepper on the spindle) but I was a bit sketical of the rpms its would achieve like 3000 rpm or so for regular facing operatiosn etc..So I decided to focus on a brushed or bldc servo with a built in tach. But you have opened up a good a new avenue, would the stepper acheive rpms of 3000?

[hfjbuis]

I use the stepper only as C-axis and it is engaged by a lever. For all other turning tasks, I use the original motor. I mounted the motor on top of the lathe, but the next build i will place it in the gearbox and use the tumbler lever (lever for changing spindle direction)... for engaging.
For drawings, information and photo's, look at:Welkom op www.mwt.messageboard.nl

I don't think you can run this large steppers that fast and still having some useful torque left. You could mount a closed loop stepper. I have never tried them but the specs look pretty good. Just for information, the first i found on google
https://www.banggood.com/High-Speed-...r_warehouse=CN

[hfjbuis]

Multi-pass threading will be implemented in the august release of the software.

[skrubol]

That's a tiny motor. I don't think .25 Nm continuous will be enough to do any real threading. According to the specs you linked, the 80W motor only has 1.6Nm peak torque. Peak torque/power, if they don't give a spec is usually only for 1 second or less. If you were planning to buy at the prices listed through those links ($150 for the motor,) it's a really poor value as well.
A large stepper could probably do what you want, you'd probably need to do about a 2:1 ratio to get the 1500 RPM output of the stepper up to 3000 though.
Something popular these days are integrated servos. They're brushless and a pretty good value.
For $300, you could get a 350 watt: https://www.teknic.com/model-info/CP..._voltage=75VDC
If that's too big, they've got a 205W NEMA 23 for a few bucks less: https://www.teknic.com/model-info/CP...del_voltage=75
People seem to like the clearpath's quite a bit and they're a good value. I think there are other similar integrated servos, but I haven't heard as much feedback on them.
Also, before you go with something that only takes step-dir inputs, make sure the controller you're going to use supports that for a spindle. Not all do, some only can do PWM (which can easily be converted to analog.)

[hfjbuis]

That's a tiny motor. I don't think .25 Nm continuous will be enough to do any real threading.

If you refer to my post, i did not specify the stepper i used.
I used a Nema 23, 2Nm stepper 57BYGH627 it has a holding torque of 2 Nm. The largest thread i did was M40 x 1.5 in Cr42Mo4 steel at 15 mm/min, depth of cut start/final 0.180/0.014 mm, 40 passes, full step, geared down 45/20.
I recently replaced it with a Nema 24, 4 Nm stepper, did the same thread at 15 mm/min, depth of cut start/final 0.220/0.021 mm, 27 passes, full step, geared down 45/20.
Consider the steppers where feed with just 13.7 Volt. So I can do threading!
Any controller can do step/dir. It is not the controller but the GCodes that make the threading. I use GRBL as controller. To do threading this way you need a 3 axis step/dir controller.
BUT you need CAM software that can do threading this way or write macro's for mach or any other controller you have.
I don't like cam for simple parts that are only made once. So i wrote my own software that communicates with the GRBL controller. It doesn't need cam and it does all the tasks you can do on a conventional lathe in an automated way.

[skrubol]

If you refer to my post, i did not specify the stepper i used.

I wasn't replying to your post, ZeroBacklash had posted a link to his 80 watt servo with .25 Nm torque.

[hfjbuis]

I was i bit agitated and in a hurry, not a good state of mind to reply.
0.25 Nm torque is not enough for threading and probably not enough for turning.