API threading on Lathe

[cadman2112]

Is is me, or does Mastercam have trouble outputting correct code for an API thread?

 

I searched and only found one thread where someone mentioned the trouble and asked if anyone else had a solution.

 

Looking at the Fanuc manuals it is requesting different information than the current thread cycles puts out.

 

Is there anyone cutting API threads using Mastercam?

[cadman2112]

No one cutting API threads?

[ReDEyZZ]

I cut lots of API threads, I pick my major Dia on the small end of taper,(using an external API as an example) calculate the minor Dia from the Depth of thread on the API spec, then calculate the Taper per foot for the specific thread, Example: 2" taper per foot is 4.731 deg. Then put the 4.731 in the Thread shape parameters area, the taper angle box is located at the bottom left of parameters page. Once you enter a value in the Taper angle box, Pick which end of the Taper is the Major Dia,... So if you are cutting an external API, Select the Major Dia at the small end and also check the area which says "Large end of taper or small end of taper"

 

If your tool is going the opposite way that you need on the taper, then put a negative value in the Taper angle box, I think an Internal API uses a negative value, an external taper uses a positive value.

 

HTH

[cadman2112]

Jarrett,

 

Thanks for the response.

 

The problem I see is we have coded these for a period of time and the machines, even the manual seems to call that on an external for example, the Major or ending diameter is what should be output on the G76 line.

 

Mastercam no matter what settings, I can not get this to output the way I Need to see it..

[ReDEyZZ]

Here is a sample from one of my programs, it has start and end point of thread, and the R value is what mastercam calculates how much to move in X.

 

This post is pretty much a standard Fanuc post with a couple tweaks, I run it on a Daowoo Puma lathe.

 

 

(TOOL - 3 OFFSET - 3)

(4 TPI EXT API INSERT )

N1(OPERATION 1)

G54

M8

M43

G97S500M04T0303

G0X2.537Z.2

G99G92X2.3181Z-2.64R-.235F.25

X2.3025

X2.2889

X2.2767

X2.2656

X2.2552

X2.2455

X2.2364

X2.2277

X2.2194

X2.2114

X2.2038

X2.1964

X2.1893

X2.1824

X2.1757

X2.1692

X2.1628

X2.1567

X2.1506

X2.1447

X2.139

X2.137

X2.137

G0X2.537

M9

G28U0.

G0Z10.

M30

[cadman2112]

Thanks Jarrett,

 

We've used the G76 to do this, I don't think I can get them to change their ways.

 

Gonna have to figure out how to get the correct coding out of the software.

[ReDEyZZ]

No problem, If I knew posts I would give it a shot for ya, but i don't. Someone will be along with the answer... fridays are always slow.

[BrianCNC]

pg76$ #G76 threading

comment$

gcode$ = zero

lrapid$

sav_xa = vequ(copy_x)

>>>> if thdface$ = zero, copy_x = thdx3$ #Changed from thdx2$ so X value in G76 line is end X--BLG

else, copy_z = thdx2$

if thdface$ = zero, copy_z = thdz2$

else, copy_x = thdz2$

pcom_moveb

 

 

It has been awhile, but I believe line #5 in the above post block is the only thing I changed to fix this.