[underdog]

Hi. Does anyone have a way that the MC Post takes care of remembering to move the turret back when going from a short shank (facing) tool to a long boring bar?

I know MC knows the next tool is a boring bar and I'd like the Post to move the turret back BEFORE spinning the turret to a long boring bar so I don't have to remember (along with everything else programmers are thinking about). When you back up 6" from the part with the facing tool and bring around an 8" long boring bar, its ugly.

Any help is appreciated.

Thanks

[g-codeguy]

What lathe are you using? There should be more than one way to achieve the desired results. I adopted Hardinge's Safe Index programs for use on all our lathes that can use them. The set-up person changes the Z-axis index position based on the longest tool. This is done in a subprogram that stays in the control and is used for every job....and every operation. The post processors are modified to output the safe index programs. Not all of our lathes use these subs. Their post processors are set up with what is hopefully an index position where all tools will clear. Once tools are installed this index position can be changed to a closer position for time savings (or further away if necessary).

I know MasterCam has a home position you can set, but have never used it. No idea how it works. Hopefully it could be output in the NC file. I've been using some of MC for a long time, but it wasn't until 2009 that the company asked me to use MC for all my programs. Before that I hand wrote programs and used MC only to save myself trig work.

I've got to be honest here....I don't understand why someone would run a program without first knowing tools would clear when indexing. How hard is it to change the index position if needed?

[GcodeEng]

Use a home position in the post

[Jim Dawson]

Pretty sure adding a G53 Xa.aaa Za.aaa before a tool change will do what you want, then a G54 again after the tool change. At least that works on a Haas lathe. The G53 uses the machine absolute coordinates relative to the home position, so you can place the carriage in a safe location for the tool change without regard to the tool offsets. Then the G54 puts the coordinate system back to WCS with the tool offsets applied.

There should be a switch in MC that would turn this feature on & off in the post setup.

[g-codeguy]

We use G53 to position the turret on our Mori-Seiki lathes. As far as I know G53 is a machine position and has no affect on G54-G59. At least least on our Moris. X and Z are always negative. This tells me G53 moves the turret that far from the home position. The bigger the Z minus number, the closer to the chuck. Z-20. is 6 inches closer to the chuck than Z-14.

[Jim Dawson]

We use G53 to position the turret on our Mori-Seiki lathes. As far as I know G53 is a machine position and has no affect on G54-G59. At least least on our Moris. X and Z are always negative. This tells me G53 moves the turret that far from the home position. The bigger the Z minus number, the closer to the chuck. Z-20. is 6 inches closer to the chuck than Z-14.

Yup, same with my lathe, home is as far from the chuck that you can move the carriage. A G53 X0.0 Z0.0 should send the carriage to the home position, at least it would on my lathe. Anything towards the chuck from there is in the minus direction in machine absolute coordinates. Moving either axis in the plus direction from the home position would run the axes into the travel limits within a very short move.

[g-codeguy]

I would try the Hardinge Safe Index programs, but the Moris weren't in my department. They are my responsibility now, but there are a few hundred programs using G53. I wouldn't want to confuse the operator.

[underdog]

All good suggestions and my thanks to everyone who replied.

For now, I've settled on using this; The front turret tools are single digit tool position numbers and the back turret (boring) tool numbers are 21, 22,etc, so I know if I'm going to a boring bar based on the tool number, so, in the MC post, I compare current tool number to last tool number and if we're going from an "under 10" tool number to "over 20", then I add 8" to the current position and reposition the carriage backward in Z before turning the turret. All other combos; front tool to front tool, back to back and back (long) to front (short) should be good.

I think its possible MC knows what type of tool it is, so you could use some code like this on single turret machines, but I could not find any keyword in the post processor book for tool type.

[Superman]

It was asked.... what machine & what control? ...... What version Mastercam ?

Hi. Does anyone have a way that the MC Post takes care of remembering to move the turret back when going from a short shank (facing) tool to a long boring bar? I know MC knows the next tool is a boring bar and I'd like the Post to move the turret back BEFORE spinning the turret to a long boring bar so I don't have to remember (along with everything else programmers are thinking about). When you back up 6" from the part with the facing tool and bring around an 8" long boring bar, its ugly.Any help is appreciated.Thanks

Safest method is to have ALL toolchanges at the HOME position.......- the operators would then customise the NC code to suit shorter cycle times for the higher job runs( there is no benefit (in time saved) in modifying a safe program for a short run..... you may save 5 seconds for the whole program, but spend 5-10 minutes doing a change & proving it off ..... and still run the risk of a major knock)

All good suggestions and my thanks to everyone who replied. For now, I've settled on using this; The front turret tools are single digit tool position numbers and the back turret (boring) tool numbers are 21, 22,etc, so I know if I'm going to a boring bar based on the tool number, so, in the MC post, I compare current tool number to last tool number and if we're going from an "under 10" tool number to "over 20", then I add 8" to the current position and reposition the carriage backward in Z before turning the turret. All other combos; front tool to front tool, back to back and back (long) to front (short) should be good.I think its possible MC knows what type of tool it is, so you could use some code like this on single turret machines, but I could not find any keyword in the post processor book for tool type.

Yes it is possible to have different toolchange positions for 2 turrets- bit harder for a single turret though, the issue is Mastercam does not check tool lengths on tools not currently used but are loaded on the turretie T1 & T3 are the first tools used but T2 is a boring bar ..... crunch- Mastercam only knows what is the current tool, & the next tool.... it is not aware that it has a turret, it seems to utilize tooling, like, from a rear magazine. Calls in a tool, put it back, gets the next... type of scenarioThere is also too many differences between what is described in Mastercam ( ie tool lengths, other unused tools in turret, etc) & how it is actually setup in the turret.- some machine controls have the ability to look at the actual tool length offsets & adjust toolchange to be at the longest setting....instead of going to HOME position The toolsetters need to plan the tool placement

[positiverake]

Just wanted to throw this out there, on the doosan lathes I run the G53 is X0 center line and Z0 is the face of the chuck so the numbers are positive I move the turret to where I want it and look at the Machine position on the position screen and use them numbers, I like the G53 as it goes to the same spot regardless of the tool and work offsets. you could use the G30 1st,2nd,3rd ref. but you gotta set them in a parameter, I did see a macro on here some place that would set them, kinda like a yasnac G51 but you better remember to set them when going from a short to a long index position. I'll stick with the G53 good luck