Ezilathe, a useful aid to lathe programming. - Page 8


Page 8 of 8 FirstFirst ... 5678
Results 141 to 152 of 152

Thread: Ezilathe, a useful aid to lathe programming.

  1. #141
    snehalharshe's Avatar
    Join Date
    Apr 2021
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    CNC lathe programming software is used to create toolpaths through G-code to operate computer numerical control (CNC) lathe machines. This allows for machine automation, where the machine cuts a part to the specifications of the input code.
    Visit https://www.sevenmentor.com/java-tra...es-in-pune.php



  2. #142
    Member
    Join Date
    Apr 2009
    Location
    Australia
    Posts
    97
    Downloads
    4
    Uploads
    3

    Default Re: Ezilathe, a useful aid to lathe programming.

    Rengan77

    I would find auto clearing the selections very annoying if I select a different tool, usually I would not want the selections cleared. If I do, the Clear selections button is available.
    When changing operation, selections are cleared IF they are invalidated. For example changing cut direction, as they will always need re-selecting.

    Snehalharshe

    And your point is ??
    .



  3. #143
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank,

    Noted on the clearing explanation. I was probably looking at only one angle. Anyway I will play around more and feedback on the operations. I finally decided on the enclosure lid that mimics industrial cnc lathe (photos attached)

    Btw regarding thread cutting features (refer to attached photos), for a sample M6x1 thread, A comparison between a reference table and Ezilathe threading feature, I noticed there are some difference between the the table (reference) 1st to 5th passes. The final pass is similar ~ 0.06 mm and also the depth of thread is different. Just wondering is my reference table in correct or there some setting that I am not entering correctly in Ezilathe ?


    thanks
    rengan

    Attached Thumbnails Attached Thumbnails Ezilathe, a useful aid to lathe programming.-img20210615210157-jpg   Ezilathe, a useful aid to lathe programming.-img20210615210211-jpg   Ezilathe, a useful aid to lathe programming.-htb1fgmoau_rk1rjy0fcq6zevvxa9-jpg   Ezilathe, a useful aid to lathe programming.-ezilathe-1-7-3-3-thread-cutting  

    Ezilathe, a useful aid to lathe programming.-thread-cutting-guide-jpg  
    Attached Files Attached Files


  4. #144
    Member
    Join Date
    Apr 2009
    Location
    Australia
    Posts
    97
    Downloads
    4
    Uploads
    3

    Default Re: Ezilathe, a useful aid to lathe programming.

    Rengan77

    Ezilathe data comes from Machinery handbook, and has been checked a number of times.
    Your data sheet refers to Inserts dedicated to a particular pitch in this case MMT16ER100ISO for 1.00 pitch only.
    This thread profile has a Flat of 0.1443mm at the root of the thread, and this is reflected in the charted values.
    You have Ezilathe set for non-std shortening of 0.00 flat (i.e. a sharp Vee tool).
    Set to Standard shortening to see the effect (Gives same depth of thread 0.6134mm)
    Also Ezilathe set for Flank Infeed - Constant Volume, not Radial infeed, so the intermediate cuts are even more different.
    Mach3 only uses Flank infeed - Constant Volume - Very Wise.



  5. #145
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank,

    Thank you for your reply and clarification. Please don't get me wrong, I trust the data in Ezilathe. I was just wondering how to make sense of it and where I need to get the correct information. I am merely a novice when comes to machining, I cherish your knowledge and experience and always open to learning from you sir. I recently acquired SER1010H11 + 11ER AG 60 Insert. Can you share how to setup this tool on Ezilathe ?

    thanks
    rengan

    Attached Thumbnails Attached Thumbnails Ezilathe, a useful aid to lathe programming.-1pc-ser1010h11-lathe-turning-tool-holder-boring  


  6. #146
    Member
    Join Date
    Apr 2009
    Location
    Australia
    Posts
    97
    Downloads
    4
    Uploads
    3

    Default Re: Ezilathe, a useful aid to lathe programming.

    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.

    Last edited by Stutank; 06-19-2021 at 05:23 AM. Reason: Clarification


  7. #147
    Member
    Join Date
    Mar 2015
    Posts
    17
    Downloads
    8
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    Rengan77 you might need more cuts, as you have limited power. I tend to increase the number of cuts until last cut depth is between 0.05 and 0.1 on steel.



  8. #148
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    Quote Originally Posted by Dragon8 View Post
    Rengan77 you might need more cuts, as you have limited power. I tend to increase the number of cuts until last cut depth is between 0.05 and 0.1 on steel.
    Hi Dragon8,

    Thank you for your input. You are suggesting the first depth of cut ?


    thanks
    rengan



  9. #149
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    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.



    Cheers
    best regards
    rengan

    Attached Thumbnails Attached Thumbnails Ezilathe, a useful aid to lathe programming.-ezilathe-1-7-3-3-od-turning   Ezilathe, a useful aid to lathe programming.-ezilathe-1-7-3-3-od-turning  
    Attached Files Attached Files


  10. #150
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    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





    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

    Attached Files Attached Files


  11. #151
    Member
    Join Date
    Apr 2009
    Location
    Australia
    Posts
    97
    Downloads
    4
    Uploads
    3

    Default Re: Ezilathe, a useful aid to lathe programming.

    Rengan77
    Note that All inputs in Red text are read only.
    Right hand window describes the thread required, so once that is set, that is all that is required for the thread parameters. Any changes on the Right hand window, sets up the cutting parameters on the Right hand window, as far as thread form parameters.
    The left hand window allows you to change the cutting parameters as required. Thread depth and infeed angle may be overridden from here. All other inputs (Black Text) can be adjusted to suit your requirements here. Mach4 only inputs are greyed out as not applicable to Mach3. Flank infeed - Constant Volume should be left as is for Mach3. Z axis feed required shows the feed needed (Green if OK, Red if exceeding system capability if entered for lathe), Easy to exceed if cutting large lead threads.

    G28 - can be an issue for some, for a variety of reasons (Yours is one I did not think about). G53 (Move to Machine Coordinates) is perfectly valid, and recommended under Mach4. Like everything (Almost) in Ezilathe, it can be altered. If you go to the Speeds / Feeds window, you will see the Lathe details on the Right hand side.
    Exit String #1 usually is set to "M5 G28" This can be set to "M5 G53 X0 Z0", "M5" or any value you require. The Homing position can be a little remote from where you are working, so can be adjusted here or in the G-code file to something more appropriate especially Z for short work. Exit String #1 is added at every Toolchange. Exit string #2 (Usually "M30") is added at program end. Also note the 3 init strings (Added at program Start) and Tool Change String added at tool change lines.

    Dragon8 - is suggesting the last cut depth. The table in the center of the threading window lists the details of the cuts you have specified. Reading the Last listed "Inc. Cut" is a good indicator as to how "Radical" your screwcutting will be. Something you will have to get a feel for, as material (Brass to hard steel), Thread length (Springing of long threads) etc. all effect the number of cuts used. Just wind up the number of cuts (Up/Down arrows just for this) until you have the required value Here. I go even further than dragon8 suggests a lot of the time, and use cutting oil on Steel. Don't stick with that chart, it is not applicable to you without coolant etc.



  12. #152
    Member rengan77's Avatar
    Join Date
    Nov 2020
    Posts
    22
    Downloads
    11
    Uploads
    0

    Default Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank,

    Sorry for the late reply. I was in the process to get the COVID shots for the entire family and had to complete my cnc mini lathe dc motor controller (clone KBIC-120/240) connections to Mach3.

    My replies to your statements:-

    "Note that All inputs in Red text are read only.
    Right hand window describes the thread required, so once that is set, that is all that is required for the thread parameters. Any changes on the Right hand window, sets up the cutting parameters on the Right hand window, as far as thread form parameters.
    The left hand window allows you to change the cutting parameters as required. Thread depth and infeed angle may be overridden from here. All other inputs (Black Text) can be adjusted to suit your requirements here. Mach4 only inputs are greyed out as not applicable to Mach3. Flank infeed - Constant Volume should be left as is for Mach3. Z axis feed required shows the feed needed (Green if OK, Red if exceeding system capability if entered for lathe), Easy to exceed if cutting large lead threads."

    Noted on the above, will be trying out soon on the physical lathe.

    "G28 - can be an issue for some, for a variety of reasons (Yours is one I did not think about). G53 (Move to Machine Coordinates) is perfectly valid, and recommended under Mach4. Like everything (Almost) in Ezilathe, it can be altered. If you go to the Speeds / Feeds window, you will see the Lathe details on the Right hand side.
    Exit String #1 usually is set to "M5 G28" This can be set to "M5 G53 X0 Z0", "M5" or any value you require. The Homing position can be a little remote from where you are working, so can be adjusted here or in the G-code file to something more appropriate especially Z for short work. Exit String #1 is added at every Toolchange. Exit string #2 (Usually "M30") is added at program end. Also note the 3 init strings (Added at program Start) and Tool Change String added at tool change lines."

    Noted on the details above. I have decided to add "M5 G53 X0 Z0" for exit string #1. I understand on what you mean if the home position is near the work piece and far away from it. Currently my mini lathe has a fixed position limit switch which is to ensure the machine does not go past its designed physical limits. However, the homing I have implemented without physical switch and use software to locate the homing within a relatively close to my varying workpieces. This ensures everytime I make a tool change, I can save some time by avoiding long distances to the homing location.

    "Dragon8 - is suggesting the last cut depth. The table in the center of the threading window lists the details of the cuts you have specified. Reading the Last listed "Inc. Cut" is a good indicator as to how "Radical" your screwcutting will be. Something you will have to get a feel for, as material (Brass to hard steel), Thread length (Springing of long threads) etc. all effect the number of cuts used. Just wind up the number of cuts (Up/Down arrows just for this) until you have the required value Here. I go even further than dragon8 suggests a lot of the time, and use cutting oil on Steel. Don't stick with that chart, it is not applicable to you without coolant etc."

    Noted on the above, I will feedback once I physically try out the screw cutting.

    I will be getting my cnc lathe up and fully operational within these few weeks. I will share the results then.

    Thank you again for your feedback and sharing your vast knowledge and experiences with me and other fellow members. I learnt alot from your replies and will be learning more once I get to physically make chips. Thank you for your superb contribution, The Ezilathe

    Stay safe
    Best Regards
    Rengan

    Attached Thumbnails Attached Thumbnails Ezilathe, a useful aid to lathe programming.-ezilathe-exit-string-png  


Page 8 of 8 FirstFirst ... 5678

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Ezilathe, a useful aid to lathe programming.

Ezilathe, a useful aid to lathe programming.

Ezilathe, a useful aid to lathe programming.