[Stutank]

Rengan77
Your 11ERAG60 is a full 60 deg insert (No Flat or Rad on Tip). setup in screwcutting with Non-Standard Shortening of Zero (As you had it setup originally)
Check tool 11 from the sample tool list (Screwcut External 60 deg) it is a 16ERAG60 insert.
Most settings are obvious, but Max cutting Depth entered as 3 sets the tool projected width, useful when cutting up to a shoulder.
16 size is 1.75 leading edge to tip (1/2 measured width of 60 deg profile). Projected width 1.75 divided by Tan(30) = 3.031.
I do not have 11ERAG60, only 11IRAG60 that measures 0.8 Projected width.

All the above does not effect screwcutting, only the visualization in the Simulator, you can see when you are clear of any shoulders etc.

Hope this is what you need.

[rengan77]

Hi Stutank,

Thank you for your detailed reply. As usual your knowledge is very much appreciated. My reply for each items as follows :-

1."Your 11ERAG60 is a full 60 deg insert (No Flat or Rad on Tip). setup in screwcutting with Non-Standard Shortening of Zero (As you had it setup originally)"

My Reply: I understand this is due to the fact my insert has a sharp tip.


2."Check tool 11 from the sample tool list (Screwcut External 60 deg) it is a 16ERAG60 insert.
Most settings are obvious, but Max cutting Depth entered as 3 sets the tool projected width, useful when cutting up to a shoulder.
16 size is 1.75 leading edge to tip (1/2 measured width of 60 deg profile). Projected width 1.75 divided by Tan(30) = 3.031.
I do not have 11ERAG60, only 11IRAG60 that measures 0.8 Projected width.

My Reply: I can create another tool 11ERAG60 with the altered geometry as you suggested.


3."All the above does not effect screwcutting, only the visualization in the Simulator, you can see when you are clear of any shoulders etc."

My Reply: I understand the visual representation on the simulation and the actual screw cutting process will move according the the tool path created by the gcode. I can physically see it on the tool path generated by Mach3 turn.

BTW I have attached several photos (Ezilathe 1.7.3.3 OD Turning and Threading 1,Ezilathe 1.7.3.3 OD Turning and Threading 2 & Ezilathe 1.7.3.3 OD Turning and Threading 4) and gcode (Ezilathe 1.7.3.3 OD Turning and Threading 3).

Do I need to alter the "Depth of Thread *, Core Diameter and Basic Pitch Diameter ? How those parameters effect the thread cutting ?

I managed to complete my cnc mini lathe connection for the optical sensor and tested the threading feature in G32 and G76. It works great as expected. The video link is below.

https://youtu.be/TNxDchyP2JI

Cheers
best regards
rengan

[rengan77]

Hi Stutank,

My questions this time is related to Ezilathe and Mach3. I managed to get my DIY 8 position tool turret working. My videos is as follows

https://youtu.be/0DbrWo-zqjE

https://youtu.be/hW2jwKpJqbo

Just to describe how I implemented the 8 position tool turret :-

1.It utilizes a Nema23 stepper motor/worm gearbox combination with no tool # 1 position sensor (purely open loop)

2.Initial position require tool # 1 to be position correctly before start of machining (MDI into position in Mach3) and reposition back to tool # 1 after machining (I added T0101 line of gcode manually in the main gcode before M30 command(refer to my gcode attached as used in the videos).

3.The m6start macro will handle tool change; by first homing X and Z axis, perform the tool change and finally updating the Mach3Turn Tool DRO once a tool change is called and completed.

I have a slight problem initially with the behavior of the tool turret when the line "M5 G28" executes after each completed tool path for a particular tool number.
When G28 executes, both X and Z axis will return to its homed position (as expected which is ok) but it will also home any other axis that is enabled, such as A-axis used for the tool turret, hence the lost of tool position.

After much trial and error I made a work around by manually substituting G28 with G28 Z0 and G28 X0, which solved the problem.

OLD CODE
*********************************

T0202 (Carving Tool - 22 deg LH)
(Process = O.D. Turning - Cut Right to Left)
M3 S600
G00 X25.0 Z0.5
(Rough #1 R-L)
.
.
G00 Z0.5
M5 G28

T0303 (55 Deg Diamond RH Face/Turn)
(Process = O.D. Turning - Cut Right to Left)
M3 S600
.
.


NEW CODE
*********************************

T0202 (Carving Tool - 22 deg LH)
(Process = O.D. Turning - Cut Right to Left)
M3 S600
G00 X25.0 Z0.5
(Rough #1 R-L)
.
.
G00 Z0.5
M5
G28 Z0
G28 X0

T0303 (55 Deg Diamond RH Face/Turn)
(Process = O.D. Turning - Cut Right to Left)
M3 S600
.
.

This definitely work well as shown in the video but I have to manually alter the codes to make it work. Also X axis actually moved to X0 (work coordinate + offset) and then move to X0 (G53) as in the video. This did not pose any issue but seems to waste some time. The behavior of G28 X~ Z~ is described in the forum below.

https://www.machsupport.com/forum/in...?topic=41827.0

"Fred,

G28 by itself in Mach3 provides for movement without axis definitions resulting in a transverse move to machine zero. As noted in Mach definitions, the intermediate point is the current point and only one movement is made when no axis words are given. One must be careful in it's use since G90, G91, and additionally Fixture Offsets can affect the resulting machine movements when G28 is commanded.

To home an individual axis, say X axis, add axis definition to the G28 command for example:

G28 X0.0 - if a G54 / work offset exists and you are away from the exact offset value then you will have two movements. IE; it will first go to the intermediate value ( the work offset value ) and then go to X axis machine zero.

G28 X0.0 – if G54 exists and you are at the exact offset value then you will have one movement ie; since your at the intermediate value there is no need to move to it so one move only to the X axis machine zero.

G28 X0.0 – if no offset exists there is no intermediate movement and the axis just goes to X axis machine zero.

G91 G28 X0.0 – there is no movement since mode is changed to incremental and the request is for zero movement

G28 – only one movement back to machine zero irrelevant if there is a work offset

Take some time and try the G28 along with axis definitions and see note the movements that occur.
Try G28 X1.0 for example and see what happens!


RICH"



Do you know any other method I can just home just X and Z without homing any other axis, as my A-axis ?

I have found using G53 X0 Z0 also works but I need to still manually edit the codes, I am ok with manual editing.

Just to share the m6start macro handling the tool change already has the ability to automatically home X and Z ( via G53 X0 Z0 within the macro itself) as long as it is called via T0x0x. This means I can actually omit G28 after M5 since the next line will the T0x0x that will automatically home axis X and Z.

Maybe this could be a suggestion for Ezilathe to be able to turn ON/OFF G28 ?

Your input is much appreciated

Cheers, stay safe and best regards
rengan