Help with chase line

[CBNDude]

This is from a fanuc 5t (old I know)..this will chase a 4.5 in. I.D. threads 2 start. 29 degree..machine compounds into thread .007 per pass on diameter and down .0009 ... I would like to know what the D stands for, and how to figure the starting Z for the deflection pass's ..

G00 X3.950;
Z1.0;
G76 X4.615 Z-4.0 K2825 D100 F1.0 A29;
G00 Z0.931;(deflection)
G76 X4.615 Z-4.0 K1500 D50 F1.0 A29;
G00 Z0.5;
G76 X4.615 Z-4.0 K2825 D100 F1.0 A29;
G00 Z0.431;(deflection)
G76 X4.615 Z-4.0 K1500 D50 F1.0 A29

Thank u in advance ------CBNDude------

[CAMCRASH]

N_ G76 X_ Z_ K_ D_ I_ A_ F_
This is a brief explination on the old fanuc style thread cycles.
The G76 command automatically performs all cutting operations required to achieve a thread. From the programmed variables the cycle will calculate the toolpaths, based on the desired thread pitch, depth, and tool angle. X designates the minor diameter of thread. Z specifies the end of the thread. D designates the depth of the first pass. K specifies the depth of the thread. F specifies the desired pitch of the thread. A is tool angle. I defines a tapper line or tappered thread. +I# will mean the back of the thread will be larger than the minor dia specified by X and a -I# will cause the back of the thread to be smaller than the mionr dia. Use I on pipe threads or on long threads to compensate for machine varience over distance.

Also I believe there are also 2 other varibles you can add to leave stock for a final pass at end of cycle and make repetative dead passes.
I will check this out on 2/18/05 and repost
I will also give an example program

GOD BLESS THE CAD/CAM
NOW THE COMPUTER REMEMBERS NOT ME.

[CAMCRASH]

I was wrong about the other 2 varibles. These are only availble in the 2 line G76 cycle

I belive if you are going to chase the thread with 2 canned cycles and you plan on changing the K value you will need to figure out the difference in the K varible over the angle specified and adjust z value accordingly to what you find
If I were to do this with a canned cycle and I needed to take out deflection.
use a G76 with a angle of zero take a smaller cut to insure tip dosent break. Then follow up with a G32 thread cycle at the same Z and use this to chase the deflection out you can repete the G32 as many times as needed.

Another option is to use the I varible to compensate for deflection if the defection is the same from part to part

I havent done this in a while and might me missing some little things so you may want to sample the above on test parts to work out the bugs.

[CBNDude]

N_ G76 X_ Z_ K_ D_ I_ A_ F_
A is tool angle. I defines a tapper line or tappered thread. +I# will mean the back of the thread will be larger than the minor dia specified by X and a -I# will cause the back of the thread to be smaller than the mionr dia. Use I on pipe threads or on long threads to compensate for machine varience over distance.

can U explain how the above works in little more detail...Thanks for ur reply I
am used to programming with chase lines like this:

G78 P_ Q_ ;
g78 X_ Z_ Q_ F_A_;

[CAMCRASH]

1" - 8 Thread Single Start

Standard start codes
Tool, Spindle Speed, Coolant, Etc.
N110 G0 X1.2 Z.5 Initial Referance Move (Clearence Position)
N112 G76 X.8492 (Minor Dia) Z-6.0 ( Length Of Thread ) I0.0 (Tapper)
K .0754 (Major - Minor / 2) Radial Distance From Minor To Major
D.010 Depth Of First Cut A60 Included Angle Of Insert Tip
F.125000 Feed Per Rev ( Some Machines Require E as Feed Call For
Thread) (Six Place Decimal)

1" - 8 Thread Double Start

SAME AS ABOVE FOR INITIAL LEAD
Then
N114 G0 W.0625 (Incremental) Or Z.5625 (Absloute)
N116 (SAME AS LINE #112 )

OPTIAN 1
If your thread is.023 smaller on diameter at the 6" dimension
Change your I0 to I-.0115 This will make the thread tapper as it travles.
You figure this by measuring the pitch at the front and the pitch at the rear of the thread take these two numbers and subtract from each other. Then devide in half. If the thread is smaller at the rear use a negative number if it is larger in the front use a positive.

OPTION 2
If the taper is caused by a Part or tool deflection you can follow up with a G32 Line (NOTE change your A60 to a A0 in the G76 line if your are not good at figuring trig formulas) A60 causes your tool to move in at a 30 Deg angle every time it takes a new pass This is to keep the major chip load on one side of the tool. Most tools cut best with a chip load on only one side of the tool. A0 makes it so the X axis will move in but the Z will not adjust at all.
After the G76 line Plce a line similar to this
N114G0 X.8492 (Rapids from canned cycle return point to Minor Dia.)
N116 G32 Z-6.0 F.12500
N118 G0 X1.2
N120 G0 Z.5
N122 G32 Z-6.0 F.12500
N124 G0 X1.2
N126 G0 Z.5
Repete as needed
You can also start above in your X axis and move down on every pass
By placing the above lines after your canned cycle it creates dead passes at the Basic Minor Diameter

If You need to make a double lead thread
Use The 1" - 8 Double Lead Lines seen above in post after the dead cuts
and once again follow up with G32 lines or adjust the I0 to compensate for pitch deviation.


Hope this helps

[CBNDude]

Perfect thanks alot..Am indeed greatful...

Thank you
CBNDude

[CAMCRASH]

correction to option #1
If the pitch diameter is larger in the rear use a positive