This hints page has been created to help you with some basics that most owners should know about their CNC machines.
These comments and suggestions should be used in conjunction with the Hercus Manual for your particular lathe.
These things work for me, it is up to you to decide if you wish do any of these things.
Getting Started With Your Machine
Safety and Lathe Stoppages
Maintenance
The PC
Software
Tools
Operation
The DOS Turret
Programming
When connecting the cables that connect the lathe to the PC, make sure the lathe is OFF and that the PC is OFF. Failure to do this can cause problems!
It is absolutely essential that the leads connecting the lathe and PC have their plugs firmly in place and that the retaining screws are tight. If any retaining screws or nuts are missing, find replacements. The behaviour of the lathe can be most erratic if these plugs are not screwed up tight.
Before You Power Up Anything!
For a machine in unknown condition, the following is important. With the machine unpowered, the operator should physically move the axes to roughly the centre of their travel. On a PC200, the axes can be pushed (with some effort) as they have efficient lead screws. On PC160’s the lead screws are square cut threads and can’t be pushed, so covers need to be removed and lead screws turned to achieve this position.
Sometimes a machine sits silently while the operator tries to get life into it, not realising that an axis has over travelled its home sensor and wedged itself into a physical end stop. In this situation the axis motors are not powerful enough to free the axis. Persisting with this may cause the motor to burn out.
To Power Up The Machine!
Always press in the Emergency Stop on the machine, before you power up the machine.
All checks in the software's Manual Page to be completed. Running a program, or even homing a machine with a fault, before doing these simple checks, results in confusing error messages.
The aim here is to asses whether the axis can be moved under the simplest of controls and that the spindle can be started. More importantly to asses nothing moves until such a move is intended.
Enter the software, turn on the machine then pull out the emergency stop button.
At this point nothing should move. If it does push in the emergency stop to prevent over travel and we suggest you contact Simon for advice. If you are able to proceed further, (assuming nothing moved) enter the manual page.
Again, nothing should move. No spindle or axis movement should take place. If it does, push the Emergency Stop back in (Power Off) promptly and contact Simon for advice.
If you have got this far you need to check that the axes can be moved via the mouse presses on the axes buttons on the screen. The software will at this point warn you that the machine has not been homed. DO NOT HOME THE MACHINE!
You need to accept this warning to proceed but DO NOT HOME THE MACHINE. Press each of the axes buttons confirming that the axis actually moves in both directions and in the correct direction for the associated action occurs.
The Manual Page shows numbers for both the spindle and axes. Confirm these are changing in response to the spindle and axis movements. If all that checks out the machine should be good for operation.
At the back of the lathe, at the headstock end are various electrical switches.
The mains on/off switch, a key which allows the machine to run with the hood up and circuit breakers for the spindle and both X and Z axis.
Only turn the lathe power on once the software is running.
The key has one position which stops the lathe if the hood is raised, the other allows the lathe to operate with the hood up. Use this with care and as appropriate.
If the lathe suddenly stops operating due to a known fault/collision, check the circuit breakers. If re-setting the circuit breakers gets the lathe going again, things should be fine provided you have fixed the cause of the stoppage.
Should the lathe stop for no apparent reason, trip a circuit breaker, and fail to start again after resetting the circuit breaker, further qualified investigations may be required.
There is also a mains fuse in the socket where the mains plug attaches to the lathe.
The DOS lathe pendant has a stop button on it. If pressed by mistake the lathe will stop. When the lathe is powered up both the red and green LED lights should be on.
If you have any doubts about the functioning of the pendant, it can be unplugged. The machine can be still operated with the mouse on screen in the Manual Page.
The Emergency Stop circuit can be a little strange if the switch needs replacing. In this condition the switch becomes very touchy and the lathe can stop without the switch being touched. I have replaced 3 switches in 3 lathes, once replaced, the lathes have worked perfectly.
The lathe has oil nipples on the cross slide and at the end of the bed. If you don’t have an oil gun, get one!! Lubricate as per the manual with lathe at HOME position. DO NOT use grease!!
When the lathe is cold, at start-up of the spindle, it is usually a while before the spindle will run at top speed, due to the headstock oil being cold. If you find the lathe is getting to high revs quicker than usual when cold, check the oil window for the headstock. The oil may be a bit low.
It takes very little oil to top up the headstock. Try just a couple of squirts from an oil can and wait awhile then check the oil window again. Too much oil is not a good idea, it tends to get thrown out of the spindle at both ends.
There is a cooling fan at the back of the machine, look at the filter occasionally to make sure it is clean.
Turrets may misbehave if swarf gets inside the covers. If you feel competent, it is worth removing the covers to remove any accumulated swarf.
To use the PC Interface card your PC must have an ISA slot. These days, they are usually only found in older style computers.
Motherboards with ISA slots are still available new but, be warned, they can be quite expensive. They are still available, because many large enterprises (like defence and mining) still depend on this older technology that uses ISA cards.
The PC requirements for the DOS software are not really that much as DOS itself runs on an older type 486 computer. To run the Windows software you will need a system suitable enough to meet the needs of W95/98.
The DOS software works well, but is perhaps not as convenient as the Windows software. In DOS, each function, e.g. Edit, Run, Manual, is entered separately, whilst in the Windows software, these functions are available in the one main workspace.
DOS
The DOS software is not impossible to use, particularly, if you use a good file manager. I use Xtree Gold. My DOS PC is setup to boot straight to the Hercus Software. I only have to use a single DOS command line to switch between the, Hercus software and Xtree Gold.
Win 95/98
The DOS software can be run in Windows 95/98 and if you set it up in Win 98 SE you can use a USB memory stick for file transfers etc.
Win 98 also gives the opportunity to load a windows based CAD if you can find one. This can be convenient if you need to re-draw the part you are making for some reason. You can then export a .dxf file straight into the Hercus directory. DOS requires DXF version 10, I think the windows software will work with version 14.
If you wish to keep text files for each job, it can easily be done using Notepad that comes with Windows from Win98 onwards.
For drilling, use stub drills (short and rigid), you may find that centre drilling is not required.
Stub drills are available as normal stub drills and CNC stub drills. You will find that while normal stub drills are not expensive, CNC stub drills can be up to five times the price, the CNC ones may be more economical for long runs.
If you need to drill deep holes, Deep Hole Jobber drills (available from Suttons) are very good for deep holes, their geometry is very different to normal jobber drills. Once again not cheap but if deep holes are required they could possibly pay for themselves. Start the hole using a stub drill of the same size and drill about 2D depth.
If you want to run a program at high speed, you should allow the spindle to warm up by running the spindle in Manual mode for a while. Either that, or reduce the spindle speed until the spindle warms up.
When threading make sure you start the threading operation well before the thread is actually required to be cut. If you want to thread at perhaps 2000 RPM and 1.25 pitch, it could possibly be up to 6mm of lead in required to enable the lathe to have the carriage moving at the correct speed to create a proper pitch thread. Doing the same thing at 1000 RPM might require only 3mm of lead in, to cut the thread correctly.
When using a single point tool to cut a thread, reduce the major diameter.
For a M10 thread, I would turn the major diameter to 9.90 before cutting the thread.
The DOS Turret is unidirectional and must be in a state of balance to work correctly. If a Hercus Boring Bar holder (cast iron) is holding a steel boring bar of any length it will be quite heavy. This weight must be offset by tools (or blanks) being placed opposite the boring bar to balance the turret. It is worth weighing these components to ensure your turret is balanced. I know this may seem extreme, but if the turret is not balanced reasonably well, you are likely to find a boring bar and its holder have not moved out of the way and will crash into the chuck or work piece.
Later turrets, driven by stepper motors do not have this problem. I think it still makes sense to have a reasonable balance in these turrets just to lower the stress on the stepper motor.
Drill or boring Bar in the turret?
When starting out, it might pay to measure the distance from the end of the tool to the turret face. Add this distance plus 20mm to the retract of all the other tools in the turret. This will hopefully ensure that the drill or boring bar will clear the work piece and chuck each time the turret revolves.
Sub Routines
Both software packages allow you to create subroutines which enable multiple parts to be run without the machine having to Home again.
The code for a subroutine is as follows:
Nxx G57 R1 where Nxx is the line number, G57 is the start of the subroutine and R1 is the number of the subroutine (you may want to have more than one subroutine). Place this line at the start of the routine you wish to run.
Nxx G58 where Nxx is the line number and G58 is the line that precedes the G59 line.
Nxx G59 R1 C100 where Nxx is the line number, G59 ends the subroutine R1, indicated by R1 and C100 is the number of times to repeat the subroutine before ending the program.
So G57 starts the subroutine, G59 ends it and the G58 line is placed on the line above the G59 line. Make sure you simulate this to ensure it is behaving as you require.
The following is an example of a subroutine to run a program 3 times:
N10 G90 G71 G95
N15 G57 R1
N20 T01 M6
N30 G50 X150.00 Z100.00
N40 S2000 M3
N50 F0.10
N60 G00 X20.00 Z10.00
N70 G00 X19.00 Z1.50
N80 G01 X19.00 Z-10.00
N90 G01 X20.00
N100 G00 Z1.5
N110 G01 X18 Z1.5
N120 G01 Z-10
N130 G01 X19
N131 M5
N140 G00 Z50
(LOAD NEW PART
N141 M00
N150 G58
N151 G59 R1 C3
N152 M2
If in doubt you can email your program to Nigel at notewell@optusnet.com.au and I will be happy to look at it for you. Please remember to tell me if it is for DOS or Windows.
Code Lines
The Hercus software requires that each line starts with an N number, but they do not have to be in order.
The software also expects to find a G instruction e.g. G01 after each N number
N50 G01 X20 Z20 will move the tool at feed rate to the position specified.
N50 X20 Z20 will bring up an error message.
The tool approaching the part.
Whether the tool is coming from HOME or from a position you have nominated you may find it helpful to bring drills and boring bars to X0 Z20 and turning tools to the diameter you want them at and Z20. This can provide just enough time for you to recognise that you made a horrible mistake when setting the G50 and hit the Emergency stop before anything nasty happens. Modify the Z20 to suit your own degree of experience, nervousness or state of terror.
The code for a tool change looks like this:
N10 G52 X0.0 Z0.0
N20 M5
N30 T01 M6
N40 G50 X163.41 Z83.49
N50 S1000 M3
When you are using a number of tools, this piece of code can be edited to speed things up.
N10 G52 X0 Z0, the first line is sending the tool to the home position. If you are happy to retract the turret away from the chuck far enough to ensure nothing goes bang, you can edit it, to become a G00 line with X and Z at positions with which you are happy.
N20 M5, stops the spindle, if you have no reason to stop the spindle, you can render the line inoperative with a parenthesis at the start of the line. Like this, (N20 M5 then the line is not seen by the machine.
N30 T01 M6, is the tool change you want.
N40 G50 X163.41 Z83.49, gives the position of the tool relative to the Home position, which of course you have to set, to suit the particular tool.
N50 S1000 M3 is starting the machine again. If you rendered N20 M5 inoperative, you can do the same for this line if you need the same RPM for this tool. The machine is still at the previously set RPM.
Reminders in the code. If you wish to make notes in the code regarding the type of tool used you can start the line with a parenthesis like this:
(55 deg tool AG insert Tool position 3
If in making a part, you require it to be loaded a certain way, you can put a reminder line in the code at the appropriate spot
(Load in chuck, large end away from chuck
I usually insert a line in the code reminding me of the position of Z, as in the DOS software you have to exit the edit function to see what it is, which is a pain.
(Z-58
To assist with knowing where you are, as the program window is quite small, it helps to use headings for each part of the program, like the following perhaps:
(DRILL
(FACE
(PROFILE
Each on a line on its own before the code you wish to label.
I usually record all sorts of notes about the program at the start of the program. I often use up to three or more lines of notes, to remind me what tool type of tool is in what position and anything else I need to know.
The code below is a part of one of my programs.
(NEW DRILL HOLDER, SHORTER DRILL NOT REQUIRED)
(6/6/08 T03 35 DEG LONG TOOL, T01 12MM DRILL IN CI HOLDER)
(DRILL MUST BE SHORTENED BY 3 MM)
(THIS IS ABOUT AS FAST AS THIS MACHINE CAN GO)
N10G90G71G95
N15G57R1
N20T01M6
N30G50X169.4Z73
N40S1750M3
N50F0.0700
N60G00X0.000Z10
N65G00X0Z5
N70G73X0Z-28R5Q8.8F.1
N71G00X2
N72G01Z-.3
N73G00Z10
(TURN)
(N111S2200M3)
N140T03M6
N150G50X114.32Z168
N170G00X27.000Z1.50F.15
N180G00X25.400Z1.500
G02 and G03 (circular interpolation) are opposite in the DOS software to the G02 and G03 in the windows software. I believe the DOS software is not as per the usual G code standard. If you own both machines the Programs can be interchanged except for the G02 and G03. If you go through the program and reverse the G02 and G03 commands, the program should work.