Hello Guest it is May 17, 2021, 02:53:21 PM

Author Topic: G73 program help!  (Read 4785 times)

0 Members and 1 Guest are viewing this topic.

G73 program help!
« on: November 26, 2013, 07:11:36 AM »
Well, I've been trying to get a G73 program to work on Mach3Turn for a couple of days - I think I'm not far off having read every post about G73 on machsupport!  Anyway, I thought I'd post the code in case anyone can spot anything obvious straight off the bat.

Here's the code:
 
G18 G20 G40 G80 G90
S3000 F65
M3 M8
T2
G0 X0 Z1
G73 X0.0 Y0.0 Z-10 R1 F65
M2 M9
M30

I have also attached a screenshot of the turn options.   All other boring and turning ops seem to be working fine.  G83 is also working fine.  G73 isn't doing anything i.e. the tool isn't moving anywhere with any of the variations of the code I've tried.    Anyone got any ideas?  Any help is of course very much appreciated. 

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: G73 program help!
« Reply #1 on: November 26, 2013, 09:14:43 AM »
Have a look at Using Mach3 Turn Manual, Page 10-15, you need a Q value.

One other thing.......The rapid backout has a setting in Mach3 Mill and not Lathe.

Don't do much cnc drilling on my cnc lathe other than some micro work using a high speed drilling attachment.
The lathe drilling macros I use can be found in Member's Doc's.

RICH
Re: G73 program help!
« Reply #2 on: November 26, 2013, 10:04:16 AM »
Rich, Many thanks for this.   A Q value doesn't seem to make any difference unfort.  I feel like I've tried every possible combination of code! It's strange that G83 works fine but I haven't got it to move at all for G73.

The point on rapid backout is very useful. The manual gives the very basics of G73 but not much beyond that. The only thing it says of use regards G73 is 'Rapid back out defined in the G73 Pullback DRO on the settings screen', which, if you're right about back out, is a very misleading statement.  Not sure which settings screen it might mean - maybe this part of the manual was written for an earlier version of Mach3Turn when there was one settings screen rather than multiple config and settings screens?  :-S

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: G73 program help!
« Reply #3 on: November 26, 2013, 11:00:08 AM »
Is there a G73 in Turn? I am thinking there isnt as no m1073 macro as far as I can see and that seems to be the way Turn deals with canned cycles. In other words there is a M1076 and a M1083 and they work, although as I discovered recently the M1083 has been replaced in later versions by a half working version.
Hood

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: G73 program help!
« Reply #4 on: November 26, 2013, 04:40:27 PM »
Hood,
I don't think there is and like yourself I checked for the M1073.mis and it is not to found under the macros used for a lathe profile.

whistule,
Let me clarify something about the macros I mentioned in Members Doc's.
They are drilling macro's to be used on the lathe when you have an actual drilling device  mounted on the crosslide.
IE; Use a high speed drill mounted on the crossslide and to  drill a series of holes in the stock face ( the macro provides for it)
of something along the X axis,rotate the spindle, drill another pattern. Whatever.

You can use them to drill a single hole using with spindle turning. I haven't used them in ages, but will say that the peck drillling
macro realy worked well. When your drilling a small hole on the lathe ( think they were .013" dia. ), spit for lubricant ???, the pecking
cycle came into play.

RICH

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: G73 program help!
« Reply #5 on: November 27, 2013, 02:56:40 AM »
The G83 seems to work well, if, and only  if, you have the correct one.
The one that has come with Mach for a while is an old one and it has issues such as the Z will feed back in after the retract rather than rapid back in.
To see if your macro is the new one open it and look to see if it has the following at the start, if not then its the old one.
Hood
Code: [Select]
'G83
'08/20/05 Edited the macro for the new engine. Brian
' March,03,05 - There was a bug with the first peck depth not working from R                   
' Feb 25 - 2005 Got the Macro working and will do a Full peck with                                               
  'C=0 and High speed peck the C=1 that will retract to the last peck depth                                                           
' Feb 23 - 2005 Added parameters and file call to Turn section                                                             
                                                             
' DRill G83 X (optional)  Z (mandatory) Q (Mandatory) R                                                 
                                             
' added tTaper to replace C parameter C will be 0 for G83, 1 for G83.1           
' Added R as peck size in G81.1     
' added check of R > StartZ for G83 
Re: G73 program help!
« Reply #6 on: November 27, 2013, 06:03:33 AM »
Very interesting responses.

Hood: Yes I'm getting exactly the same with the G83 - feeding all the way with no rapids.  Good to see someone else from Scotland on here - I'm just doon the road in Glasgow

Rich: Good clarification - I see you're talking about active tooling.

It does all point towards there being no G73 in Mach3turn - even if its inclusion in the manual would suggest otherwise

It does seem there are some fairly big omissions in the current version of mach3turn -  mainly the lack of programs G70-73.  I'm only just beginning with it and seem to be bottoming out all over the place - so I'm sure there other powerful programs missing that I don't know about.  But in terms of adaptability, even just missing G70-73 is crippling in terms of how powerful CAD-CAM is.  I'm wondering if these are ever likely to be developed in future versions or if this territory is just going to be left to CAD-CAM from now. 

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: G73 program help!
« Reply #7 on: November 27, 2013, 06:11:56 AM »
Ok you need the newer G83 macro, I can either attach it later or you can download an old version of Mach and install it on another computer and grab the macro.

I have a friend in Glasgow that is doing a lathe soon, Mount Vernon area.

Hood

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: G73 program help!
« Reply #8 on: November 27, 2013, 07:42:35 AM »
Hood,
When you get a chance just attach it and I will put in Members Doc's.

Thanks,
RICH

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: G73 program help!
« Reply #9 on: November 27, 2013, 08:18:33 AM »
Here is the macro


THIS REPLY MODIFIED BY RICH 11/27/2013:
Here is a link to the macro in Downloads > MACK TOOL BOX. There are other macro's in the tool box that may be of interest.

http://www.machsupport.com/forum/index.php/topic,25976.msg183054.html#msg183054
« Last Edit: November 27, 2013, 05:30:34 PM by RICH »