Denford Software & Machines

Hi,

I know that this is going to sound really lame, but could someone please post a correct GCode program for the Orac for thread cutting?

The reason I ask is that I am very green with these machines, and when I try the threading, sometimes it works brilliantly, and other times the tool digs deep into the workpiece at the stsrt of the cycle and breaks the tip

I think that I am inputting the program correctly but can't be sure.

I am trying to cut an M18x1.0 thread, and have all the correct pitch threading tips etc.

I am fairly sure it will be an error that I am making, and not the machine at fault, hence the seemingly lame question

Any help would be much appreciated.

Thanks
Paul

Why not post the program that you're trying to run, someone might be able to spot the error (if any).

cheers,
v

Hi Paul

Are you using maximum spindle speed for the thread pitch ?
If not could be the tool digs in because there is low torque from the motor and the
spindle stops turning but the Z axis keeps moving, this would cause tool tip damage.
This is more of a problem with coarser threads where max spindle speed is really low,
(90 rpm for a 3.0mm pitch)
For a 1.0mm pitch max spindle speed is 280 if using Denford program so perhaps you
need to reduce the depth of cut per pass to reduce chance of "digin".

Which program are you using to write/edit and load a program to the lathe ?
or are you entering direct at the lathe control panel.

Rgds, Emgee

Hi,
I am using the lathe control panel to input the program, as it is the only way that I know how.
I was using the 280RPM for speed, which I got from a thread cuting graph.
I am unsure if I am entering the program correctly as I dont really understand the "program datum" values, and I'm not sure if I am entering the program in the correct sequence of commands.
I have tried to find information online for the correct way to input the program, but have drawn a blank.
I think the way I did it was:
Page 001 Metric units
Page 002 Absolut/Incremental format (tried both)
Page 003 Program Datum
Page 004 G33 threading program
Page 005 End program.

I believe that I have set the tool offsets correctly.

Thanks

If it sometimes works brilliantly and sometimes digs in on the first pass it would suggest the tip is either not repeating back to the same X position, or the blanks are a different size ?
Check for repeatablility on the X axis - eg, rapid back to home and then return to a known position (eg onto a dial-test-indicator)
then repeat, maybe adding a few short moves at different feeds. If it isn't repeating then check the home switches (if any) and check the slideways, ballscrew and pulleys for tightness.

Hi

If the program and tool datums are not the same when the program starts the tool will be move by the amount of difference between the 2.
At page 3 enter G50 and set X 00 and Z 00, tool rubbing corner of workpiece.
After entering the program go to manual mode to position the tool rubbing as above, depress the Em
STOP and use the manual buttons to bring the XZ display both to 0.000, (with the stop depressed the axis won't move.)
Release the Em stop and press the small manual Stop, this will return you to the choice scren on the VDU.
Use execute program and press enter, screen should show both axis at 0.000, press manual stop (not Emergency Stop) and Tool offset choices are available, take your pick of the options, if you use all tools set at X00 Z00 you won't encounter problems in a program using only 1 tool. Tool No.1
After setting the tool offsets press F1 and the program will go to page 1 and follow codes entered.
Will post a program later.
Rgds, Emgee

triac wrote:Hi

If the program and tool datums are not the same when the program starts the tool will be move by the amount of difference between the 2.
At page 3 enter G50 and set X 00 and Z 00, tool rubbing corner of workpiece.
After entering the program go to manual mode to position the tool rubbing as above, depress the Em
STOP and use the manual buttons to bring the XZ display both to 0.000, (with the stop depressed the axis won't move.)
Release the Em stop and press the small manual Stop, this will return you to the choice scren on the VDU.
Use execute program and press enter, screen should show both axis at 0.000, press manual stop (not Emergency Stop) and Tool offset choices are available, take your pick of the options, if you use all tools set at X00 Z00 you won't encounter problems in a program using only 1 tool. Tool No.1
After setting the tool offsets press F1 and the program will go to page 1 and follow codes entered.
Will post a program later.
Rgds, Emgee

Hi, Thanks for taking time to write that, an example program would be great

I will digest that then have another try

Thanks

Hi Paul

Go to here https://www.denfordata.com/pdfs/Orac-Pro ... es-OCR.pdf (ORAC Forum page)and download the manual, all you need to know is contained therein. For your guidance the program below will do the 18x1.0mm thread 20.0mm long with a .50 thread depth.

p01 G71 mm
p02 G91 incremental
p03 G50 X00 Z00 (make sure in manual mode tool shows X00 Z00 position)
p04 M03 spindle on
p05 G33 threading
in/out diameter 18.00 (outside thread)
Root diameter 17.00 (for 0.50mm depth of thread)
Cut (inc) X .03 (depth of cut per pass)
Length Z 20.00 (change to suit your length)
Pitch 1.0
Starts 1
Tool No. 1
Spindle speed 280 (max for 1.0mm pitch)
p06 M05 spindle stop
p07 M02 program end

Before entering this turn your bar to 18.0mm diam with a .75mm chamfer, position your threading tool rubbing the end face and at 18.0mm diameter.
Rgds, Emgee

triac wrote:Hi Paul

Go to here https://www.denfordata.com/pdfs/Orac-Pro ... es-OCR.pdf (ORAC Forum page)and download the manual, all you need to know is contained therein. For your guidance the program below will do the 18x1.0mm thread 20.0mm long with a .50 thread depth.

p01 G71 mm
p02 G91 incremental
p03 G50 X00 Z00 (make sure in manual mode tool shows X00 Z00 position)
p04 M03 spindle on
p05 G33 threading
in/out diameter 18.00 (outside thread)
Root diameter 17.00 (for 0.50mm depth of thread)
Cut (inc) X .03 (depth of cut per pass)
Length Z 20.00 (change to suit your length)
Pitch 1.0
Starts 1
Tool No. 1
Spindle speed 280 (max for 1.0mm pitch)
p06 M05 spindle stop
p07 M02 program end

Before entering this turn your bar to 18.0mm diam with a .75mm chamfer, position your threading tool rubbing the end face and at 18.0mm diameter.
Rgds, Emgee

Awesome, thankyou very much.

I will try it out the next time I get a minute.

Very much appreciated

Paul