Hello

I was trying to cofigure Mach3 for my new router. After a couple of hours I typed G0X1. The axis moved 2,5 cm - that is one inch. Im a metric user so I`ve change on top of the Config menu from inches to millimeters. A massage came up, that its only for motortuning, but i`m not shure what it means.  It doesn`t change anything. It still moves 25mm. My machine needs 500 step to move 1 millimeter. Thats what I wrote in the Motor tunnig menu.

Then I loaded a Gcode of a Nameplate that is 150mm wide, but on the display it was probably wider then 1000mm - it was outside my table and larger then my router. I suppose I can se my table size because I`ve type the software limits?

What am I doing wrong?

Adam

I think you have your ****** in a twist. You must decide BEFORE you do anything else whether you are a metric or imperial user. This does not mean you cannot work in the other dicipline if you want to, it means that mm or ins is the unit in which your whole system is set up. I work in steel, and if your move G0X1 resulted in a 25 mm move, then I would be in trouble - an inch is 25.4mm. It may not mean anything when you are routing wood, but if you were in steel it is the difference between a fit or not, by a wide margin (16 thou to be precise)

What you must do is set up your units first. Then set up your motor tuning - i.e. the steps per unit. Since I do not know your machine, I must assume that your calculation of 500 is correct. On my steel lathe, it is 1200 but I have a 3 to 1 reduction, so your 500 sounds about right.

The speed and acceleration are for setting when you are satisfied your steps per unit is correct, but for now, something like a speed of 250 per min (very conservative) and acceleration of 50 will do, and will not lead to any missed steps.

If you now check your machine, input g21 - (metric), then G0X1 and your axis should move 1 mm. If you enter G0X25 it should move 25. If you enter G20 (imperial) then G0X1 it should move 25.4mm (not 25).

If you are not correct with your movements ( and make sure you always measure in the same direction ) i.e. move the axis right, zero the DROs then move right again and measure - (to avoid backlash) then you must check your steps per unit calculation. I don't think you are so far off.

Do not try to adjust the steps per unit figure to make the movement correct - it is a finite figure that depends on the geometry of your machine, and cannot alter. If you are getting wrong figures, the fault must lie elsewhere.

I think you shift between metric and imperial on the setting page.

In the lower right corner you have a button "Units Alt-U". Hit it and the metric/imperial led turn on-off. See what you have there.

Thank you for your anwers. I will try that. But my router is located 35 km away from my apartment and internet, where my friend is building the router for me.  There is only home and limit switches left, thats why I´m using the software limits. I`ll try again next weekend.

But is it true that the only place where you can type the table size is in the software limits menu? Just so I can se where the material is located on my table.

Adam

The tool display does not show the workpiece. It shows the outline of your program. We must assume you will put the workpiece in the correct place.

This may be the time to explain the difference between Machine and Program Co-ordinates, if you are fitting limit and home switches.

Mach 3 keeps track of your machine in Machine Co-ordinates. You can look at the Machine Co-ord DROs by pressing the Machine Co-ords button on the screen. The led surround will light. You cannot alter these co-ordinates, and you have no control over them. The only way to affect them is to "home" your machine. The machine will move to the home switches, one by one, and then stop. The DROs will set to zero (if you have the auto zero ticked). This is the only way to alter the Machine Co-ordinates.

Mach now knows exactly where the machine is.

It is not likely that the position of the "home" switches will be in a convenient position to work from, and will certainly not bear any relationship to the program you are running.For this, you use program co-ordinates. Program co-ordinates are determined by the program, either one you have written, or one a Cad/Cam program has written. This will have a 0.0.0 position for the three axis. For different programs, the 0.0.0 position may be different, depending on size, layout, thickness etc. and you must look at your machine and table, and work out the best place for your workpiece, and where the 0.0.0 position is on it. It may be a small piece, in which case you may decide to use the centre of the table, or one corner. It may be a large piece which overhangs the table.

The general start point for programs is X0 Y0 to be the bottom left hand corner, with Z0 as the cutting tool just touches the top of the workpiece. This is a general thing, but not necessarily so, and your 0.0.0 position can be any where.

If you are doing a large number of the same piece, you will probably have so jig attached to the table, so that each work piece will be in exactly the same position.

How do you marry up the Machine Co-ordinates that the machine knows, with the program co-ordinates ? The answer is offsets.

If you "home" your machine, and then press the Machine Co-ordinates button, the led will go out. The DROs are now displaying Program Co-ordinates. When you first start the day, these may, or may not be the same as the Machine Co-ordinates. If they are not already at zero, you now press the zero X zero Y and zero Z buttons, the Program Co-ordinates will go to zero. If you check with the Machine Co-ordinates, these should also be zero. If you now check Config/Fixtures you will see a table which sets out offsets. When you are first starting they should all be zero. You will fill the table gradually.

If you now jog your table to Program Co-ordinate 0.0.0 position and press the zero X zeroY and zero Z buttons again, the program co-ordinates will zero. If you check the Machine Co-ordinates they will not have, and the display shows the offset for that program. If you check Config/Fixtures you will see that G54 has altered, to reflect the offset. You can use G54, but this is the default offset, and if you are wanting to use the offset in a program, you will be better to copy the figures to a different offset (g55 to g59 - and 250 sub sets of g59 - so there are plenty to go at.

If you choose shall we say G55, then you enter this is your G Code program as a line, near the begining of the program. Many programs include G54 (the default) so you can instead alter this to your program offset.

How does this work?.

"Home" your machine. Run the program into Mach 3. Lay your workpiece in the jig. Press the Cycle Start button.  The machine knows where it is, becasue you homed it. It knows the offset to the program and picks up the offset value from the table, and then moves to the new "start" position and gets on with the job. You sit back and have a cup of coffee. When the machine has finished, put another workpiece in the jig, and press cycle start again. Have another cup of coffee.

You need not "home the machine" before every cut, only at the start of the day (things may have moved slightly when the machine was turned off) or if you think somethings has gone wrong, i.e. a tool broke or the cat got stuck in the machine or something. If you suspect the machine has slipped, then you "home" it to put it back on track.

Each program can have a different offset - there are 255 to choose from, or if you use a jig to locate the work, then you can use the same offset all the time.

Hope all this makes a bit of sense.

Hello jimpinder.

It makes sens :-) 
You wrote a few things I didn`heard before in the tuturial videos. Thanks.

I will print this page and take it with me.

Adam

I suggest you also print, or buy a copy of the printed, Install Manual The complete sequence of setting up a machine is detailed very well.

See the downloads tab at teh top of this page.