Help and advice for Denfords lathe control software VR Turning.
Moderators: Martin, Steve, Mr Magoo
-
TimPower
- CNC Apprentice
- Posts: 37
- Joined: Thu 27 Apr , 2006 17:19 pm
Post
by TimPower » Thu 27 Apr , 2006 17:25 pm
Hi there folks,
I ran a program on the VR turn which worked fine but when I tried it on the machine which is a Denford Novaturn it couldn't get past the first G01 command.
The start of the program I used is below,
N10 [BILLET X25 Z45
N20 G21
N30 G99
N40 M06 T0505
N50 G97 S1500 M03
N60 G00 X27 Z2
N70 Z-0.5
N80 G01 X-1 Z-0.5 F1.5
but it just hangs on this line at the Z-0.5
Can anyone tell me if there is anything in the parameters that I need to change to engage cutting operations.
Any hints or tips would be welcome.
Best regards,
Tim Power.
University College Cork.
-
Denford Admin
- Site Admin
- Posts: 3634
- Joined: Fri 10 Feb , 2006 12:40 pm
- Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
- Location: Sunny Brighouse
-
Contact:
Post
by Denford Admin » Fri 28 Apr , 2006 9:09 am
A mistake I've made myself a few times
- the Feedrate is not set until the next block (N80) - if you ran another program that set the feedrate up, it would probably work then. Try putting an F1.5 on the end of
N70 Z-0.5
I've also been caught out with feed per rev mode as well (G99) where I've tried to move the axes in G01 before starting the spindle -nothing happens as there is no spindle rpm for the feedrate to get its speed from.
I'd also recommend updating to the latest version which you can download from
www.denford.co.uk - technical support page
-
TimPower
- CNC Apprentice
- Posts: 37
- Joined: Thu 27 Apr , 2006 17:19 pm
Post
by TimPower » Fri 28 Apr , 2006 10:34 am
Unfortunately that wasn't it, tried that but no luck for some reason. I also tried putting F30 after the S1500 to set up a feedrate. I was sure what you said would have done it as it makes sense but no joy.
Can you think of anything else I could try?
Best regards,
Tim Power
-
Denford Admin
- Site Admin
- Posts: 3634
- Joined: Fri 10 Feb , 2006 12:40 pm
- Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
- Location: Sunny Brighouse
-
Contact:
Post
by Denford Admin » Fri 28 Apr , 2006 10:40 am
I take it the rapid move does work ?
If it does then try turning off feed per rev mode (G99 to G98) and put in say a feed of F200
If all else fails - update to the latest version - I seem to think there where some similar problems a long time ago with the software.
-
Steve
- CNC Guru
- Posts: 1432
- Joined: Tue 21 Feb , 2006 16:15 pm
- Location: Denford UK
Post
by Steve » Sun 30 Apr , 2006 22:33 pm
If you start the spindle in manual mode is the spindle speed discplayed in the control panel?
It may be you have a problem with the spindle encoder not reading the speed and the program is in feed /rev.
As Denford Admin suggests try changing the program to feed / Min and see if it works then.
Also if that does not work can you also include the next few lines of code as the problem could be further down the program even though it stops at line 70.
-
TimPower
- CNC Apprentice
- Posts: 37
- Joined: Thu 27 Apr , 2006 17:19 pm
Post
by TimPower » Tue 02 May , 2006 13:13 pm
Thanks folks.
The change from G99 to G98 sorted it out but I'll download the latest software aswell because I can't cut threads with a G98. The speed is coming up on the screen so I'm assuming the encoder is okay.
Thanks to both of your help,
Hopefully I can sort the rest of it over the next few days.
Rgds,
Tim.
