Lathe bore question

[Columbo™]

I have a boring bar the I am using to rough the back wall of a bore using "ROUGH" then using the same bar to finish the bore diameters and back wall of the bore using "FINISH"..... I also have the retract set to the last move of the first operation and the approach set to the same values for the second operation.

 

My question is "why does the boring bar come out of the hole then goes back in....I have done this in the past without any issues.....Is the problem using a rough and a finish operation for the same tool????

 

Thanks

[Ron Branch @ Verisurf]

Is it in the posted code? Sometimes I see tools shows things on the screen in latha and not post them that way. Look at that real close. Check that you are not using Ref points outside the part. I have used ref point at the end of one operation and then at the start of another to keep the tool inside of a part.

 

HTH

[Columbo™]

Yes Ron.....it's posting that way also.....

 

 

My tool leaves off at D.7997 Z-2.380 but comes out to Z1.250

 

Also my retract on the first operation matches the approach of the second operation.......

 

Never seen this before......

 

 

Here is the two operations posted

 

N10 CLEAR

N20 DEF WORK

N30 PS , [0,0], [,]

N40 END

N50 DRAW

 

N60 G50 S400

 

(ROUGH FACE BEFORE SMALL BORE)

N70 G00 X30. Z80.

N80 G96 S400 M03 T0505

N90 G00 X.8123 Z1.25 M08

N100 Z-2.2729

N110 G95 G01 Z-2.3729 F.006

N120 Z-2.65

N130 X.6635

N140 X.5221 Z-2.5793

N150 G00 Z-2.275

N160 X.9612

N170 G01 Z-2.375

N180 Z-2.65

N190 X.7923

N200 X.6509 Z-2.5793

N210 G00 Z-2.275

N220 X1.11

N230 G01 Z-2.375

N240 Z-2.65

N250 X.9412

N260 X.7997 Z-2.5793

N270 G00 Z-2.38

N280 Z1.25

(FINISH SMALL BORE)

N310 Z-2.38

N320 X1.09

N330 G01 Z-2.48 F.016

N340 Z-2.625

N350 X.8035

N360 Z-3.08

N370 X.7328 Z-3.0446

N380 G00 Z-2.38

N390 X1.15

N400 G01 Z-2.48

N410 Z-2.655

N420 X.8635

N430 Z-3.08

N440 X.7928 Z-3.0446

N450 G00 Z1.25

N460 G00 X30. Z80. M05

N470 M02

%

[calnet42]

I have sent this problem into Mastercam via my reseller.

I am still using X2 Mr2 Sp1 for all my lathe programs specifically because of this problem.

 

When switching between 2 sequences, the tool is forced to retract to the stock face plus the tool clearance dim.

 

I was given a work-around which works sometimes but, I have not yet recieved a "fix" for this.

[Columbo™]

Thanks Calvin......thought that it might be a bug.....I don't do to many lathe programs but I don't remember that issue.....

 

Thanks

 

[calnet42]

No problem, I have been waiting for someone else to mention this, I thought it was me.

[calnet42]

I just found a possible answer to this problem.

Here is the link...

Linky

Check out the posts from Bob Hendrick.

 

I un-checked "write home position clearance moves" and all the extra z rapids are gone.

 

You MUST use reference points to control entry and exit moves wnen this is off but, I use them anyway.

 

See if this helps.