More questions about cnc setup

[binfordw]

1. I'm a bit in the dark about home switches. I understand limit switches and why they are used, but what about home switches? In the Mach3 software it says home switches arent required- how do you zero things out without them? Will I really be fine without using home switches for now?


2. Spindle motor control. I havent seen/read anything about spindle control yet. Will I have to manually turn on the spindle and set the speed before running programs? What is required to allow mach3 to control the spindle speed?


thanks

[John Stevenson]

1. I'm a bit in the dark about home switches. I understand limit switches and why they are used, but what about home switches? In the Mach3 software it says home switches arent required- how do you zero things out without them? Will I really be fine without using home switches for now?

In Mach one of the limit switches can be doubled up as a home switch. It's then personal choice whether you use them.
Some go to home then work from there, some register on the vise or part and call this the origin 0,0.



2. Spindle motor control. I havent seen/read anything about spindle control yet. Will I have to manually turn on the spindle and set the speed before running programs? What is required to allow mach3 to control the spindle speed?


thanks

You need a breakout board that can handle spindle speed, it takes in a signal from Mach which sends pulses to the spindle part of the breakout board.
This then sends out an 0 -10 v analogue signal that the machines spindle speed board can understand.

One thing to watch though is that many of the Chinese machines with DC motor have the speed controls at mains potential and the speed part of the break out boards MUST be isolated completely from the rest of the system.

.

[jacampb2]

I too was confused about this when I first was researching my Mach3 retrofit on my b'port. I ended up making one limit switch home on each axis, and checked the function, it worked, after initial setup, I have probably not once "homed" the axis', as John says, touch off or indicate the part, zero each axis and run the code. Depending on the size or design of the machine, it might make sense to home the axis', but I have about 36x18 inches of travel for x and y, that would leave me making most part on one corner of the very extreme end of the table.

For a small bench top mill it might make more sense, or for a gantry style sheet machine, it makes a lot of sense, but for mill work, not so much IMO.

Later,
Jason

[binfordw]

Thanks for the replies that clears it up pretty well.

I guess the spindle control isnt a big deal. Ive never run one of these small machines so Im just not sure how everything goes yet. My only experience has been running larger machines at my previous job.

[macona]

I too was confused about this when I first was researching my Mach3 retrofit on my b'port. I ended up making one limit switch home on each axis, and checked the function, it worked, after initial setup, I have probably not once "homed" the axis', as John says, touch off or indicate the part, zero each axis and run the code. Depending on the size or design of the machine, it might make sense to home the axis', but I have about 36x18 inches of travel for x and y, that would leave me making most part on one corner of the very extreme end of the table.

For a small bench top mill it might make more sense, or for a gantry style sheet machine, it makes a lot of sense, but for mill work, not so much IMO.

Later,
Jason

If you are not homing at startup then you are not using your machines to its fullest. Having a home switch allows you to do so much more. With a home switch you machine knows exactly where it is every time you start the machine. It also allows you to use soft limits where you tell the machine the extents of the axis travel and it will stop the machine from traveling past its limits. Really, hard limits should only come into play when there is a problem so bad that you have a runaway axis and the hard limits kill everything. Commercial machine will do absolutely nothing until you home them.

Having home at one end of the table does not mean you have to work on that end. That what G54 fixture offsets are for. On my mill I have homes at the ends of each axis. First thing you do is home the machine. With G54 set my Mach knows that the left corner of the fixed jaw on one the first vise is at so many inches from the x home and so many inches from the y and that spot is 0,0. So every time I turn on the machine and home it I can do a G00X0Y0 and the center of the tool will go exactly centered above the corner of my vise every time within a few tenths which is the repeatability of the limit switches. It saves a lot of time not having to put in an edge finder and locate home every time.

Then with G54 set you can use more offsets like G54.1, G54.2, etc and do multiple parts in the same vise with the same code by just calling the new offset before the code. One job last year I was running 4 vises on my tooling plate to minimize tool changes. Worked great!

Another advantage of having and using the homes and using offsets is if something happens and you loose position you can just re-home the machine and you will be back up and running. This can really come in handy if you are unfortunate enough to run a stepper based machine.

With a lathe you can have all your tools set in the tool chart for tool offsets. When you call the tool it compensates for the length and offset from one side to the other. I can have my lathe off for months, turn it on, home it and run a part without doing anything more than loading stock.

As for your spindle it is going to depend on what kind of motor you have. If it is a DC motor in a chinese machine then you need either a pwm or step-dir isolated analog converter to drive the speed control. If it is an AC motor you will either have to change it to a DC motor and drive or a 3 phase motor and use a VFD and drive that with the same step/dir or PWM to analog converter. I like the digispeed series from Peter Homann at http://www.homanndesigns.com I have his boards in just about every CNC machine I have built.

In the I/O area in mach there are settings for the spindle options. You can choose between step/dir and PWM. They both will work equally well. Mach also allows closed loop spindle operation where you put something like an encoder or retroreflective sensor on the spindle and the machine will sense how fast the spindle is running and adjust it for load. Its also pretty handy just to be able to see how fast the spindle is running.

[Dawai]

My opinion...

Well... the Limit switch.. it shuts down the hold coil in the "ESTOP" MASTER RELAY circuit, stopping all motors, stopping the spindle.. whoaa.. no gooa NO Mo till reset..

I have a mushroom estop, in series with the limit switches, you must hold the reset to get it off a crashed end limit. End limits are there to protect ballscrews. They should be adjusted to the point where they can stop a full G00 Move before it crashes to the end.

A home switch however can be software directed. I am not saying you should do every machine like I do all of mine.. but I got all my fingers. I do not depend on Bill Gates or any other lil bits of software magic including my own. Computers get confused. Heck I get confused.

THE spindle.. well.. I got a manual switch in the inverter 24 volts, it looped through a relay controlled by the software, and the mechanical spindle brake is all manual.. if I leave it applied, as I have before while changing tooling, it holds and trips the inverter out..

Problems? well breakoutboard pin status? I was working next to the cnc, the power blinked, the computer reset, rebooted, the spindle turned on.. Well.. the odds may be 1,000 to 1 that I would be changing a end mill at that exact time and space.. but.. I'd have it heavy on my mind each time I did so. MY MCR does not "turn on power" till I push the reset..

If you want to get fancy? take your keyboard emulator and have it throw a ~ sign to the software to reset the software estop also.. (Mach3)..

Write all your setup information down. I recently had to go back to Geckos on two axis.. and had to recalibrate them all over again.

[Dawai]

HOME location...

my cnc bridgeport has a lil notch in the table, in that notch is a hole, to absolute the "mill head" location..

You tram the mill, home the "table" then swivel the head around and locate the "HOLE" with a probe ... that locates the table to "run" programs you set up before.. then you raise table to "touch off" and set Z depth.. Once you build some decent programs of things you make more than one of, you'll find that endmills constantly change diameters and lengths.. to do a circular bore job with a endmill as Mach3 is great for (3" hole with 1/2" end mill") measure your end mill and enter that into the setup wizard there.. end result will be exact... close enough to run a small piston..

I keep saying I will build a endmill table to set the mills up as per instructions and software design.. but.. I don't do that much repeat work.. I am great at making scrap from good steel and aluminum.