multi start thread

[Thoob]

Hi guys. I am wondering if there is a way to set my multi start to not offset on each start. Reason I ask is because I am trying to do grease grooves but it has to be like a multi start thread except for the offset on the start. Can I set it different? I notice in the parameters, there is no such option.

[Brad Lisle]

I have not tried this yet but try coping thread op and then change thread start position this might start at a different angle. You would have to manually calculate the proper distance if it is at a specified gap.

[Thoob]

Ok I posted out the program with default settings. The cycle is posting out something I'm not familar with. Can someone identify this code for me? The G0W.0588 move. What is that code? That an incremental move on the z?

 

G76P000060Q20R0.

G76X3.075Z-4.4688P625Q80R0.F.11765

G0W.0588

G76P000060Q20R0.

G76X3.075Z-4.4688P625Q80R0.F.11765

G97S136M03T505

Z-4.4674

G76P000060Q20R0.

G76X3.075Z-.4688P625Q80R0.F.11765

G0W-.0588

G76P000060Q20R0.

G76X3.075Z-.4688P625Q80R0.F.11765

[steveo25]

Ok I posted out the program with default settings. The cycle is posting out something I'm not familar with. Can someone identify this code for me? The G0W.0588 move. What is that code? That an incremental move on the z?

 

G76P000060Q20R0.

G76X3.075Z-4.4688P625Q80R0.F.11765

G0W.0588

G76P000060Q20R0.

G76X3.075Z-4.4688P625Q80R0.F.11765

G97S136M03T505

Z-4.4674

G76P000060Q20R0.

G76X3.075Z-.4688P625Q80R0.F.11765

G0W-.0588

G76P000060Q20R0.

G76X3.075Z-.4688P625Q80R0.F.11765

 

Yes "w" is incremental in Z and "U" is incremental in X

[Thoob]

Yes "w" is incremental in Z and "U" is incremental in X

So if I was to just remove that W, would that eliminate my multi start offset?

[steveo25]

So if I was to just remove that W, would that eliminate my multi start offset?

 

Do you have access to a programing manual for this machine. If you look up the G76 cycle it will break it down for you. What type of machine is it? I have several fanuc manuals right here.

[Thoob]

Its a Romi M20 fanuc series 21i-T

The incremental move is only when I select multi start.

[steveo25]

Yea it looks like the "W" will just offset the tool after the cycle is ran. So if you removed the "W" it will run the same cycle as the previous. Are you doing spiral grease grooves?

[Thoob]

Yes I am. But will it make 2 threads 180 degrees from eachother still?

[steveo25]

Yes I am. But will it make 2 threads 180 degrees from eachother still?

 

Your feeds and speeds are calculated based on the length of the groove from front to back. So taking the offset out WILL throw the timing off.

 

We do grease grooves all the time. We load these sub programs into the machine and have the main program call them up

 

%

O1000 (GROOVE SUB 1) first groove starting towards front of part

N1000 G32 U0.300 F3.064 <----calculated by length of groove times 2

N1005 G32 W-1.532,<-----length of groove towards chuck

N1010 G32 W1.532<------ length of groove back to front of part

N1015 G32 U-0.300

N1020 G00 U0.007

N1025 M99

%

 

%

O2000 (GROOVE SUB 2) second groove starting towards back of part Same as up top but reversed

N2000 G32 U0.300 F3.064

N2005 G32 W1.532

N2010 G32 W-1.532

N2015 G32 U-0.300

N2020 G00 U0.007

N2035 M99

%

[Thoob]

Ok Thanks. I'll try that procedure out.

[steveo25]

Ok Thanks. I'll try that procedure out.

 

The structure of the program looks like this

 

(.250 WIDE FULL NOSE RAD I.D. GROOVE)

G50 S1118 M42

G55 G00 X0.0 Z0.0 T0 M08

G97 S26 T0808 M03<-------rpm is calculated by 140 divided by feedrate

G54 X2.444 Z1.0 <---"x" move is .300 under the finish dia of the bore

Z-.484 <---First start point

M98 P1000 L20 <---call up 1st sub program and repeat 20 times

G00 X2.444

Z-5.04<------Second start point

M98 P2000 L20<------call up 2nd sub program and repeat 20 times

G00 X2.444

Z1.0

G97 S799

G55 G00 X0.0 Z0.0 T0 MO9

M01