Rich!!---right now I  have a full blown obstacle with the interference issue that has surfaced...see my new post on my Frankenstein moment...As soon as I've got that cleared up, then I will get back to your lessons...bob

Rich hi... solved the vfd issue by installing a new shielded cable... problem solved.... so I will work on your lessons now.   bob

Bob,
Glad you got it fixed and on the first try.

#4
The 4th axis or rotary defined in degrees is used for indexing.
If verticaly mounted you could move way from the center of the rotary to some location drill a hole , index some angle and drill another hole. When mounted horizontaly you are still indexing.

The rotation of movement + or minus , cw/ccw, is defined by mathematical standards and the Right Hand Rule is good way to remember it. Direction of spindle rotation is the same as the mill, namely, one views from the spindle towards to the chuck in the direction of the axis.

Say you wanted to drill the holes in the quitar bridge, relative to the top of the bridge without removing  it  from the holder. Index 90 degrees and while in that position  run the code for drilling the holes.

Do the following commands using the MDI in the order shown. BUT
On a piece of paper write down what you think the motion will be and what  the dro
will show for position. And if you want to take this a step further do the same for  Machine Coordinates and  also Work Coordinates along with G90 and G91.

G54
G94
G90
G0 A0
G0 A10
G0 A-10
G0 A0
G91
G0 A0
G0 A10
G0 A-10
G0 A0
G0 A360
G0 A720
G90
G0 A1.5
G0 A0
G91
G0 A1.5
G0 A-1.5

The way the rotary rotates to get to a position and what is also shown in the DRO
can be affected by "Rotational"  settings. Config>General Logic Configuration has three Rotational settings you can use.

Rot 360 rollover – if checked the A axis DRO will display from 0 to 360 degrees and then start over at 0. If not checked the A axis DRO will be additive such that 2 revolutions will display as 720 degrees. The rollover only works for G91.

Ang Short Rot on G0 – The axis will move in the shortest possible move to a new position. So if at 0 degrees, and you jogged  to 359 deg then it would just rotate  -1 degree.

Rotational Soft Limits – if checked will apply software limit switches to the rotary axis.

You don't have any of these settings selected and suggest you try some commands
with the Rot 360 rollover and Avg Short Rot on G0 selected.

To be continued,

RICH

Bob,

#5

CNC Cookbook Site has a lot of info about CNC. Bob Warfield has number of articles
about the 4th axis. I think you will find them informative.

4th Axis Basics: What They Can Do
https://www.cnccookbook.com/cnc-4th-axis-introduction/

4th Axis for the IH CNC Mill
Spread sheet calculator for the 4th axis
http://s3.cnccookbook.com/CCMillCNC4thAxis.htm

CNC 4th Axis Basics: Workholding
https://www.cnccookbook.com/cnc-4th-axis-basics-workholding/

CNC 4th Axis Basics: Routers and Woodworking
https://www.cnccookbook.com/cnc-4th-axis-basics-routers-and-woodworking/

Mill Turning 4th Axis on Hobby CNC Machines
Videos of Steve Simpsons workon the 4th axis
https://www.cnccookbook.com/mill-turning-4th-axis-on-hobby-cnc-machines/

---------------------------------------------------------

You mentioned that the  school uses a Haas mill. Here is a link to a workbook
located in Members Docs so you can compare Mach3 commands to Haas commands.
 
GCODE PROGRAMMING REFERENCE
http://www.machsupport.com/forum/index.php/topic,24580.0.html
HAAS Mill PROGRAMMING WORKBOOK.pdf

----------------------------------------------------------

An excellent comprehensive guide to programming is CNC Programming Handbook

by Peter Smid. I highly recommend it often to folks.

------------------------------------------------------------

To be continued,

RICH

Bob,

#6

More general preparation before the fun realy starts!

It is important to understand the difference between 2D and 3D work.
The following link to Shopbot site  provides insight on  the topic.
http://www.shopbottools.com/mProducts/3-d_work_v2.htm

--------------------------------------------------------------------------------------------------------
All the lessons posted are rather focused on general awareness about the 4th axis.
So felt I should make an important comment about my lesson postings in this thread.

I am very focused on the basics relative to Mach3 and simple gcode commands which
directly relate to using a 4th axis. CAD / Cam, other gcodes, setup, etc will be ignored
as much as possible.  Just not possible to cover all in a thread, or said differently, not going to
write a book. So just understand the thread  is not in any way "all inclusive".

That said,

-----------------------------------------------------------------------------------------------------------

Mod's were done to your profile to avoid having to deal with setup issues.
A... PITA.... with the generic mill screen in that it's hard / not possible to reset Machine,
Work, and Work offset  values to zero. ( not the case with the lathe screen  though)

So attached the attached Macro will do it.
The macro  will zero out both machine and work coordinates for the X,Y,Z,A  axes and get rid
any G54 Work offsets for the same axes.

Just download the macro, rename it to M1000, and then copy it to the Mach3 directory.
To use you just type M1000 into the MDI line.

To be continued,

RICH

I got the Smid book, so I will look at that.

Great on having the book.

Just note that most of the Gcode "dialect" is Fanuc based, which Mach4 is based on.
Some commands are not supported by Mach3, but, the simple ones are the same.

For the depth that the book and many others cover, few get into 4th axis or rotary work.
You also will not find anything on the G93 mode.

RICH

Bob,
#7
                                                                                                                               -
So you did some basic G0 ( rapid moves) for the A defined as angular to see the how coding affected rotational movement. The following requires review  before doing  rotary moves at a some feedrate.

Co-ordinated Linear Motion  
------------------------------------------
 - each axis moves at constant speed and all axes move from their starting positions       to their end positions at the same time, also defined as control the axes so that, at         all times, each axis has completed the same fraction of its required motion as the        other axes.
 - IE; any two axes ( x,y or z ) produces motion in a straight line
 - the motion can be done at prevailing or rapid feedrate and may default to the slower     axis feedrate

Controlled Point
----------------------------
Definition is 7-2 and 10-1 in the mill manual.

The controlled point is the actual cutting point of the tool.  So often we envison the axis motion resulting from a given line of gcode and  forget that motion is all about moving a specific "point". The software controller controls just that point relative to the  defined motion.The material removed on the work can be very different than just an imaginery small point machining a piece.

ROTATIONAL RADIUS / CORRECTION DIAMETER
-------------------------------------------------------------------------
The following is from the mill manual and one should be aware of the Mach settings.
Click the Settings ( Alt6) tab to see them located in the upper right corner of the screen.

6.2.2.5 Diameter/Radius correction (page  6-3)
---------------------------------------------------------------------
Rotary axes can have the approximate size of the workpiece defined using the Rotational Diameter control family. This size is used when making blended feedrate calculations for co-ordinated motion including rotational axes. The LED indicates that a non-zero value is defined.

6.2.12 Rotational Diameter control  (page 6-11)
--------------------------------------------------------------------
As described in the Feedrate control family, it is possible to define the approximate size of a rotated workpiece so the rotational axis speed can be correctly included in the blended feedrate. The relevant diameters are entered in the DROs of this family.

The Axis control Family has warning LED(s) to indicated the setting of non-zero values next to the axis DRO in the screen.

Values are not required if rotary movement is not to be coordinated with linear axes. In this case a suitable F word for degrees per minute or degrees per rev should be programmed.

MY COMMENTS
- Available in the mill screen only.
- Above settings apply to Feedrate description #3.

Feed Rate Modes
---------------------------
There are 3 feedrate modes and they are  described  in Section 10.7.27 on page 10-28 of the mill manual. Below are sanitized descriptions.

G93    - inverse time feed rate     - F = 1/Fnumber in  minutes ( if the F number is 2.0,                                                              the move should be completed in half a  Minute)
                                                        - very infrequently used
                                                        - if active, an F word must appear on every line which                                                           has a G1,G2, or G3 motion
                                                       -  an F word on a line that does not have G1, G2, or                                                                G3 is ignored.
                                                       -  does not affect G0 (rapid traverse) motions.
                                                       - It is an error if: inverse time feed rate mode is active                                                          and a line  with G1, G2, or G3 (explicitly or implicitly)
                                                         does not have an F word                          

G94   - units per minute feed rate   -  F= inches / minute, mm / minute, or degrees /                                                                      minute,  determined by length  units are being
                                                               used and which axis  or axes are moving

G95    - units per rev feed rate         -  F= number of inches / mm per degrees per                                                                         spindle revolution, determined by what length
                                                                units are being used and which axis or axes are
                                                                moving.
MY COMMENTS                                                                    
- Note that for the lathe, mode  is usualy G94 and changes to G95 for  threading.  
  
FEEDRATES 1. & 2.
---------------------------------
There are 4 descriptions about how Mach interprets  feedrate described in Section 10.1.6 of the mill manual when in the >>>>>> G94 <<<<<<<<  feedrate mode. Below are sanitized descriptions.

    
1. A or B or C (only one axis)                  - no X,Y,Z movement          F=degrees/min

MY COMMENTS
- Rotation of one axis at max velocity (as defined in motor tuning for the axis) you            simply code: G0  A 360.
  There is no feed rate "F" since by definition of G0 it is a "rapid" move. Additionaly
  the degree value would be positive or negative to define the rotational direction. The
   A value is the number of degrees to rotate.
  
 - To rotate the axis at different feedrates one would need to add the feedrate  and            also use G1.

    G1 A360 F3600
    The F value in degrees per min relates directly to the velocity setting in motor
    tuning. If velocity setting is 3600 and it represents a table rpm of 10 rpm, then  a
    feedrate of 1800 would move the table at 5 rpm.  

  - One should test at different feedrates, record the actual rpm, and make a graph for
    later use.

  - Re read  the  Feed Rate Modes for defintion of G94 and read 10.7.1 and 10.7.2
    in the  manual.

  - Compare the descriptions  of 1. and  2. ( below )

  - An axis becomes irrelavant to this command if it's used as slaved axis for a gantry /
   router type  machine.
  
  - The attached file  pertains to my rotary index. You may want to do similar for your
     lathe.  


2. X, Y, Z  + A, B, C     -  WITHOUT simultaneous rotation -    F =length / minute  ( along
                                                                                                      the linear  path)  

G1 X1 Y1 F100

MY COMMENTS
- actual length of the above linear move depends on current location and what mode
  is active. ie; G90 or G91, the modes and feedrate remain in affect until changed by
  gcode

- Machine Coordinates always show absolute location from zero reference

- feedrate may default to max velocity of the slower axis if coded F number is higher
  for the other axes

NOTE: The next lesson #8 and maybe #9 will address the other two feedrate modes.

             Lesson 7 coding exercise is an attachment to this reply.

To be continued,
RICH

Rich--I am at the phase of uninstalling ver. 066 and putting in ver .062 per your or others recommendations.  I don't remember having to put in a access code etc..  Is there a way to find my code on the current version, so that when I install ver .062  I wont have an access problem??  bob

By code I assume you are meaning your license file that was sent to you.

Save your xml file ( contains configuration you used ). I also would recommend that you save and keep you license file some place safe. Install ver 062 and if asked also install LazyCam. Copy the xml file and license file to the Mach3 directory. No harm in running the drive test after the installation, as that will that will install the driver. ( been a while and just don't remember exactly)

When you open Mach3 you can check under about that it is registered to you. You can also scan the settings and motor tuning that they are correct.

RICH