Hello Guest it is May 27, 2019, 05:43:23 AM

Author Topic: Lathe Turn wizard question  (Read 4392 times)

0 Members and 1 Guest are viewing this topic.

Lathe Turn wizard question
« on: January 21, 2008, 09:39:52 PM »
WHen I generate code with the the lathe turn wizard the infeed of the x-axis to the cut depth is a G0 command which is just fine when the tool is out beyond the end of the stock (Z+** ) But when the z start point is a Z negative value it would be nice if the wizard would generate the x axis infeed line as a G01 instead of G00 ., It would also be nice if the x ais infeed speed could be specified as a seperate value from the z axis feed value. On short files I have just been editing this manualy but today I generated a file to cut profile a large mortar bbl thats aprox 4000 lines with almost all the x axis infeed commands being at a z negative position. Is this an easy option to add to the turn wizard? thanks
Re: Lathe Turn wizard question
« Reply #1 on: January 21, 2008, 11:09:09 PM »
If Z0 is the end of your stock, why would you want to start the cut IN the stock instead of Z+ just a tad ?
Which one of the wizards are you referring to ?
RC
Re: Lathe Turn wizard question
« Reply #2 on: January 21, 2008, 11:37:36 PM »
The OD Turning wizard is the one I am referring to.  On most parts I turn I do start off the end of the stock in Z+ but a few things I have turned recently , like AK gas pistons and today a large mortar bbl have had a somewhat wasp-wasted profile and I need to start in the part somewhat. Some of the firing pins I turn are rather small in diameter and I have to support the end away from the chuck with a live center and start turning Z- of the end of the stock to leave a short portion of the original stock for the live center to bare against, Simply not possible to start off the + end of the stock. When the tool plunges into the work piece at 150 IPM in rapid it causes the part to deflect , this wouldn't be to big a problem if there was a dwell or pause before the movement in the z plane to allow the tool time to remove some stock but the way it currently works it rapids in to the cut depth and them instantly begins to travel in the z- direction. When this happens the part just deflects and ends up larger in diam away from the chuck than closer or just breaks the tool.

My thought was for the x axis to rapid (G00) in as long as the Z start value is + and feed in at a user definable value (G01 F**) if the Z start is negative , Maybe what I am looking for exist in one of the other wizards, unsure, but it does seem it would be a useful addition to the OD turn wizard since it not feasible to rapid in on the x axis in every situation

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: Lathe Turn wizard question
« Reply #3 on: January 22, 2008, 01:24:03 AM »
I know what you're saying. You are sort of pushing the edge for this wizard, this is really a reentrant cycle you need here. At the risk of being repetitive about this issue, I have been asking for a wizard that works like the G71 lathe roughing cycle a Fanuc has. It will rough to an arbitrary shape, which could easily be a DXF profile, etc. or a section of G code that is called out after the wizard. For a true reentrant shape you would need the G73 cycle which just moves the cut path in the X axis only. You might try getting hold of a CAM program, usually expensive, and even the high end ones are very lame with lathe uses, amazingly enough as a lathe is only a 2D machine. I guess even the CAM companies don't bother too much with lathe as about all machines have some version of a G71, sadly with Mach, you don't.
       DaveA.
Oh, I have a good 20mm round program for a Lahti, maybe Solothurn but it uses the G73 cycle. Sigh.

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: Lathe Turn wizard question
« Reply #4 on: January 22, 2008, 07:02:49 AM »
Whilst I don't know what your finished part looks like, I would try and write my own wizard.

If you use Vis Basic, you can quickly write a program to  thin down your stock to a working diameter, put on rounded ends etc etc,

My manual page, on Mach 3 Turn,  has now several other DRO,s available into which I can enter parameters such as starting diameter, finish diameter, length, etc etc. I have written several macros which take information from this page, and then turn the stock down to these parameters.

Roughing down to a diameter is easy, since you can use  such commands as  "While Dia > Finish Dia" etc  "Take another 20thou off".

If you send me some idea of what you are doing, I'll try and put a little macro together for you. 
Not me driving the engine - I'm better looking.

Offline poppabear

*
  • *
  •  2,231 2,231
  • Briceville, TN, USA
    • View Profile
    • S S Systems, LLC
Re: Lathe Turn wizard question
« Reply #5 on: January 22, 2008, 08:43:04 AM »
Ok,

   Here is a MOD to the Turning screen set for OD turning.  You fill in the DRO for -X Feedrate, IF your Z Start is also negative.
I posted a screen shot of the screen here and the Screen set themselves. NOTE: It will overwrite the current turn sets, but will only add in
the DRO and code nessessary to auto change to a user defined G1 if Z start is less than 0.

NOTE2: You will have to drop the "Turning.set" into the Turning Wizard folder under the "Turn Addons" folder, copy and paste it in, it will
ask if you want to overwrite the current turn set. (IF you want, rename the Original Turn set, to something else so you can go back to it
if you dont like something).

Scott
Commercial Mach3 & Mach 4, Design/Build/Retrofit CNC and Industrial machines.
http://www.ss-systems-llc.com/
Re: Lathe Turn wizard question
« Reply #6 on: January 22, 2008, 05:33:00 PM »
thanks Thats exactly what I was hoping for

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: Lathe Turn wizard question
« Reply #7 on: January 25, 2008, 11:06:08 PM »
Scott, thanks for the turning wizard. I loaded it today and tried it, but the X feed in feedrate box won't accept a feedrate. You click on it and type a feedrate in, hit enter and it goes back to zero.
DaveA.
Re: Lathe Turn wizard question
« Reply #8 on: January 25, 2008, 11:13:20 PM »
its working fine for me, it will only accept feed values for x axis infeed feed rate when the z start point is a negative value which should be the only time its needed

Offline DAlgie

*
  •  304 304
    • View Profile
    • Algie Composite Aircraft
Re: Lathe Turn wizard question
« Reply #9 on: January 25, 2008, 11:23:10 PM »
Ahh, I'll have to try it that way, thanks.