What's new
What's new

Multi Start threading

localbiker

Plastic
Joined
Nov 18, 2022
Hello , I am a new machinist/Turner looking to widen my skills and have started learning multi-start threads ,
Today i was Cnc Turning a multi-start as practice, Does this code look correct ?
As my first attempt at a Triple start did not go as planned ,
M24 * 3 N3
G0 X24. Z9.0 (Z12) - (Z15)
G76 P0201060 Q150 R0.025;
G76 X21 Z-30.0 P1840 Q250 F9.0;

I would finish the cycle then run the program with altered Z values,
Am i giving the machine enough Z distance to sync ? ,

I started by turning a m24*3 Nut+Bolt .Thread To ensure depth was correct Then simply changed material , + Altered the program Feed and start points.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
So would that be Lead/Pitch , 3/3 =1 ?

You have specified a Lead of 9.0 (F9.0) in your first post, therefore, the Pitch of the Thread is 3.0:
Pitch = Lead/Number of Starts
3=9/3
3.0mm is the distance you have to move the Z Start for each Thread Start.

Depending on the Control you have, but with a Fanuc control the Multi-repetitive Cycles can be set to Single Line Format (FS15 Format) via parameter. With the Single Line G76 Cycle, you can start at the same Z Start Point for all of the Thread Leads and index the Start with a "Q" address. If "Q" is omitted from the Command Line, Zero Degree is assumed by the control. For the remaining two Thread Starts, 120 and 240 degrees would be specified with the "Q" adress, with the Z Start Point remaining Constant.

The Two Line Format you're using is referred to by Fanuc as Standard FS16 Format and indexing the Lead Starts with "Q" is not possible. However, when the control is set to Standard FS16 Format, Multi Start Lead Threads can be cut with Threading Cycle G92 and G32 using the "Q" address to index the Start of each Lead.

Regards,

Bill
 

maguilera

Plastic
Joined
Jan 4, 2022
I would finish the cycle then run the program with altered Z values,
What you could do instead is call G76 three times with the same exact parameters, only changing the Z start position.
Am i giving the machine enough Z distance to sync ?
As stated by angelw, only for very low RPM’s. I would at least double the Z start position.
I would also change the X start position to something like X30. It’s not a great idea to keep the X starting point the same as the nominal diameter of the thread.

Cheers
 

localbiker

Plastic
Joined
Nov 18, 2022
Agree 1000%
What you could do instead is call G76 three times with the same exact parameters, only changing the Z start position.

As stated by angelw, only for very low RPM’s. I would at least double the Z start position.
I would also change the X start position to something like X30. It’s not a great idea to keep the X starting point the same as the nominal diameter of the thread.

Cheers
Sitting about 750 RPM ,
What is the reason for such a distance , Im aware it is to be safe/Precautious but other than that ?
 

sinha

Stainless
Joined
Sep 25, 2010
Location
india
In the middle of G76 execution, feed hold may cause interference with the workpiece while retracting, if sufficient X clearance is not provided.
 

sinha

Stainless
Joined
Sep 25, 2010
Location
india
With G71, X clearance should not be provided, as it would result in lower DOC than that specified, in the first roughing pass. Too large a clearance may result in air cutting for initial few passes.
Adequate Z clearance must be provided.
 

localbiker

Plastic
Joined
Nov 18, 2022
So i include safe clearance in the X diameter because :
When i feed hold, The tool will move in X away from the thread so it does not cut/Contact the material.
Unlike G71 the tool will sit at the same X-Position.
Thank you i will keep this principle in mind.
(for internal it will be lower than X but not to much or eles tool will hit workpiece.)
 








 
Top