559,610 active members*
3,524 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Uncategorised CAM Discussion > Ezilathe, a useful aid to lathe programming.
Page 9 of 9 789
Results 161 to 172 of 172
  1. #161
    Registered
    Join Date
    Dec 2015
    Posts
    9

    Re: Ezilathe, a useful aid to lathe programming.

    I have just set up a Taig Turn CNC lathe and found EziLathe. Fantastic program and the videos you did really help with using it. I've done some air cutting so far.

    This may have been answered somewhere, but I couldn't find it (and I'm no expert on CNC programming, but do OK with my CNC mill.....lathe is a new beast for me). I'm doing some conventional cutting (tool on the front side) then centre drill and drill; no problem so far. Then I want to part off with a rear tool post. Is this done in EziLathe somewhere or in Mach3? I want just the parting to be with the rear tool post without changing spindle direction (tool is upside down).

    Thank you very much for this excellent software!

    Rick

  2. #162
    Registered
    Join Date
    Apr 2009
    Posts
    108

    Re: Ezilathe, a useful aid to lathe programming.

    Carbuilder.
    Glad you like it.
    Rear toolpost - Not much in the mach3 manual, but without trying it myself (No rear Toolpost), I would try this, as a place to start. Cannot see any issue (Axis limits should be OK), but certainly keep air cutting until certain.

    1) Touch off tool as normal, but touch off at rear, and enter as negative size. This should give correct X0.0 position. Z as Normal.
    2) Change Ezilathe Parting off routine (In Favorites) as listed below to come from Rear. Note negative X, and adjust to suit your lathe/tooling.
    3) Copy / Paste from favorites into your Gcode, and adjust to suit the actual job.


    Parting off (Select 1 tool only. Change S, F, X and Z)
    T1818 (Parting Tool blade 1.5mm)
    T1919 (Parting Tool carbide 1.5mm)
    T2020 (PARTING TOOL)
    M03 S****
    G00 X-20.0 Z2.0 (Move to safe traverse Position)
    G00 Z-24.0 (Move to required Z)
    G01 X1.0 F30.0 (Part off through center)
    G00 X-20.0 (Move Back Out, Just in Case)
    G00 Z2.0 (Move to safe position, before Home)
    G28 M5

  3. #163
    Registered
    Join Date
    Dec 2015
    Posts
    9

    Re: Ezilathe, a useful aid to lathe programming.

    Thank you very much. That worked perfectly! Mach3 does have the "rear" tool option in setting up the tool table, but I found that messed things up when all the other tools were front mounted. So I just left it as front mounted in the tool table (even though the parting tool is rear mounted) along with the other 3 front mounted tools.
    Took a long time to get the tool table all set up. I don't really know why, but it seemed to mysteriously change after entering values and then going back and checking. No doubt it was because I was doing something wrong. I found the best way was to get it close, then 0,0 the main tool (#1), then use T0202 X0, see where it ends up and make adjustments in the table. Repeat for other tools.

    I did quite a bit of air cutting, then with a plastic rod, and finally last night with steel. The cutting went perfect, the parting off.....not so great. Spindle speed too fast and by time I grabbed the oil it was too late. So some adjustments needed to that; pause the program so I can swap the belt to slow down the spindle. Soon I'll be cranking out parts! My wife never believes me when I say that. These parts I need are only .2" diameter and .5" long. She looked at one and said "how much did it cost you to make that?".

    Rick

  4. #164
    Registered
    Join Date
    Apr 2009
    Posts
    108

    Re: Ezilathe, a useful aid to lathe programming.

    Carbuilder
    Glad that worked for you, might have to look at a rear Toolpost sometime myself.

    As for setting up a Tool table, A couple of comments, all tried and tested.
    1) Master tool - best a RH Face/turn tool.
    2) Using mach3 Turn.PDF - Good explanation of this (Chapter 7), Including swapping from Front - rear Toolpst in setup not recommended! Probably should have Greyed out the button.
    Basically I follow what is written in the PDF. Jpg attached is my Tool Table, slight differences to chap 7, but clearer, especially the touchX/TouchZ button locations. Note that this window does fill in the Tool Table Editor. Mach3 asks to update on exit if any changes made, so changes should not be lost. (On a clean exit).

    3) After Homing. Face/Turn using master Tool T00 or T01. Set X DRO to measured Size (Dia or rad depending on Mach setting Diameter or radius mode). Set Z to 0.0 when faced. These surfaces are now used to "Touch off" other Tools.
    4) In Part Zeroing Coordinates Dro, Enter the measured X size, and Z 0.0 before moving the relevant axis. If using a drill shank to roll through as a touch off point (eg a 3mm Drill Shank) add the required offset i.e. X Measured size + 3 rad or 6 dia, and Z 3. Note this works well, and very easy to judge.
    5) Call up Tool required and touch off Z. Finish by Pressing the "TouchZ Button" This should Enter a Z offset in the Z offset box, and the Z Dro should now reflect the actual Z touch off point as per master tool. Do the same for X, and you are set.

    I hope this helps, I've been doing this for years, and only when there is a change to a tool, do I need to repeat.

  5. #165
    Registered
    Join Date
    Apr 2009
    Posts
    108

    Re: Ezilathe, a useful aid to lathe programming.

    Sorry, Forgot the JPG of My Tool editor window (Later version than the Manual????)Click image for larger version. 

Name:	Toolset.jpg 
Views:	0 
Size:	52.5 KB 
ID:	478458

  6. #166
    Registered
    Join Date
    Dec 2015
    Posts
    9

    Re: Ezilathe, a useful aid to lathe programming.

    Don't know why I had so much trouble setting the various tools. Part of the issue is not paying attention when you go out of the tool setting window and then go back into it that you may not be on the tool you left; resets to tool #0 often.

    I also found that I would set everything up, machine the part, and it wouldn't be quite the right size. Supposed to be .155" dia and would be .162". So I tried tweaking the tool wear setting and sometimes it would change the part and sometimes it wouldn't. Then I noticed that it was also changing the part zero for the X-axis; wasn't sure if it should be doing that or not. Anyways, it took a lot of tweaking (and learning the ins and outs of mach3 turn) to finally get it to do what I wanted. It is strange that the program I put in had the final machining at .155" dia and with X0 set perfectly I wasn't always getting that. I found the best way to make an adjustment was to measure the part, say it was .160" dia, then move the X0 .005" on dia and re-zero it at that position.

    Once I finally got it all set up the parts came out perfectly and with amazing repeatability. Like to .0001" diameter.

    So with these done, and with full confidence (always a dangerous thing to have!) I'm moving on the the valves now.

    Thank you once again for the program and the support.

    Pictures show the tools ready to go; cutting, centre drilling, drilling, parting. 16 parts in less than an hour (not counting the debugging weeks).

    Rick


    Attached Thumbnails Attached Thumbnails Screen Shot 2022-04-09 at 1.37.24 PM.jpg   Screen Shot 2022-04-09 at 1.37.38 PM.jpg  

  7. #167

    Join Date
    May 2022
    Posts
    1

    Re: Ezilathe, a useful aid to lathe programming.

    So is this software only going to work with DXF files created from AutoCAD? Please help

  8. #168
    Registered
    Join Date
    Apr 2009
    Posts
    108

    Re: Ezilathe, a useful aid to lathe programming.

    TimRC
    Ezilathe should be able to process All ASCII (Text) DXF files created with any CAD system.
    Having said that, DXF files continue to develop, if you do find a DXF that does not work, I would like to know about it.

    Ezilathe only supports (or Needs) only Lines,Arcs,Polylines and LWPolylines (Also Circles for mill work).
    Splines are not supported, and should not be used, other un-supported entities are just ignored.

    Hope this helps.

  9. #169

    Join Date
    Nov 2020
    Posts
    24

    Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank,

    I just logged in after a long time. My CNC lathe conversion is almost completed. I was ill a while back so had to stop work. I needed to machine some parts to complete my CNC lathe and decided to complete my other CNC project a CNC router. I hope to make some chips soon.

    Cheers

    rengan

  10. #170
    Registered
    Join Date
    Apr 2009
    Posts
    108

    Re: Ezilathe, a useful aid to lathe programming.

    Rengan77
    Hopefully a good outcome soon. I've been doing other things recently, so no updates finished as yet.
    I've been building a CNC cam grinder (see photo) that needed software written.

  11. #171
    Member
    Join Date
    Oct 2021
    Posts
    3

    Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank. I just found out about your software, I absolutely love it! Works like a dream on our Kia Kit30B
    Dan Gray
    http://siderealtechnoogy.com/SLO/

  12. #172
    Member
    Join Date
    Oct 2021
    Posts
    3

    Re: Ezilathe, a useful aid to lathe programming.

    Hi Stutank. I just found out about your software, I absolutely love it! Works like a dream on our Kia Kit30B
    Dan Gray
    http://siderealtechnoogy.com/SLO/

Page 9 of 9 789

Similar Threads

  1. Lathe programming
    By mcm1961 in forum Haas Lathes
    Replies: 3
    Last Post: 08-20-2021, 02:35 PM
  2. Cnc Lathe Programming
    By millmonkey1 in forum Employment Opportunity
    Replies: 5
    Last Post: 02-04-2011, 01:17 PM
  3. Programming a bar puller in X2 on a lathe
    By bob1112 in forum Mastercam
    Replies: 1
    Last Post: 01-06-2009, 05:05 PM
  4. lathe programming learning ?
    By pit202 in forum Haas Lathes
    Replies: 13
    Last Post: 11-23-2007, 02:41 PM

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
  •