Tutorial Mach 3

[JAZZCNC]

Hi Richard,

Sounds to me like you have few conflicts happening here regards what Mach3 does exactly and what's needed or invloved with running and getting machine to do what you need. Because I'm build machines for people who often are brand new to cnc I see this often.

I'll try to help here and break it down excuse if you know this but feel free to contact me via PM if want to know more. I'll gladly give you my number and can chat if you like.

Ok well First Mach3's role is often misunderstood. Common for people to think it does more than it really does.
It's only purpose is to handle the Motion control side ie: Tell motors how far to travel and respond to any actions thru Inputs/outputs. ie Estop, limits and turning on spindle etc.

The problem comes from when Mach 3 isn't correctly setup. You are experiencing some of this with wrong Z axis travel.
However when correctly setup there is very little to learn or do in Mach 3 other than Set the WORK ZERO for each Axis and Press Cycle Start.

The setting up is easy enough but will require some information about your machine. ie: Screw pitch and Micro stepping set on drives along with any ratio that may be applied via timing belts etc.
Also the Pin numbers that any Inputs/Outputs are using ie: E-stop.

The actual using of Mach3 regards cutting and the Coordinate system is actually very easy to grasp when it's explained.

What you need to understand is that you have two coordinate systems working together.? MACHINE coordinates and WORK coordinates.

MACHINE coordinate ZERO is fixed and never changes unless the HOME Switch is moved. MACHINE ZERO is Reference point that all other WORK coodinates are Referenced from.
When you HOME the machine in Mach3 think of this has defining the work envalope of your machine always having fixed set point to start from.
This is done using the RefAllHome button.
Even if you have no HOME switches pressing RefAllHome will set the MACHINE ZERO at the location machine was when pressed. However caution is required here because very easy to crash machine if the MACHINE Zero is set near the limits because the WORK coordinates may run past the end of machine.

WORK Coordinates relate to the actual part. When you program the part in CAM software you will define a ZERO point on the part to start from.
When you place material on the table it can be anywhere you like. You then define WORK Zero at some point on material. Doing this creates a WORK OFFSET which is relative to MACHINE ZERO. All moves in WORK Coordinates are then done relative to this WORK Zero point.

This is done in Mach3 by clicking Axis ZERO buttons next to the DRO's showing coordinates. ie: X Zero, Y Zero, Z Zero.

After this is done then really the only thing left to do is push Cycle start. Mach then runs thru the G-code and handles the motion control.

The Importance and point of MACHINE Zero is so that if for any reason position is lost while cutting ie: Estop or tool breakage you can always easily get back to WORK Zero by Returning to the MACHINE Zero (home position).
Mach3 keeps the WORK OFFSET stored so can easily get you back into correct postion to carry on.

You can also have many WORK OFFSETS, known as Fixture OFFsets each with there own unique WORK Zero but's that's getting deep so won't go there now.
99% of users never even now they are using a WORK OFFSET because by default mach3 and most CAM packages use default WORK OFFSET called G54. Mach can use 255 WORK OFFSETs.!!

So that's MACH3 it does nothing but controls the machine and eat's G-code.!

The G-code you feed Mach can be obtained in many ways. Simplest form is by hand coding but the easy route is to use Cam Package to generate the G-code.
Each CAM package will take CAD File and let you choose cutting stratergies to achive your finished part. This is done by using the geometry of the part and then assigning toolpaths with all the appropriate speeds, feeds etc needed for your tools. ie: Drilling, Profiling etc.

All these Toolpaths(or singularly) are then post Processed into one large G-code file which you load into Mach3. The Post processing portion is very important because there are many types of CNC controls on the market with Mach3 being just one very small fish.
So it's important you choose Post processor designed for Mach3 other wise Mach won't be able to understand what's being told. Think of it like speaking differnet langauge, you need post that speaks Mach3.

So has you see Mach3 when setup isn't very complicated to use and doesn't take much learning. Taking the time to Understanding the Coordinate systems and how they interact helps clear lot of the Fog for most users.

After that it really is just Load the G-code file, Set Work Zero's and Push Cycle Start. When tool change Occurs just change tool reset Zero for Z and carry on.!

Feel free to ask any questions no matter how stupid you think they may sound.

Cheers
Dean.