Cycle time in SET file

[Henk]

My millplus post from inhouse supports a couple of custom drill cycles for 'circle milling', 'thread milling' and 'gun drilling'.

Now i want to add them in my setup sheet, an customized mill.set.

 

For the descriptoin of those operations i changed and added some lines:

 

 

 

 

 

#Select drill operation note

sdr00 : "G81 " #drill - no dwell

sdrd0 : "G81 " #drill - with dwell

sdr01 : "G83 " #peck drill - no dwell

sdrd1 : "G83 " #peck drill - with dwell

sdr02 : "G83 " #chip break - no dwell

sdrd2 : "G83 " #chip break - with dwell

sdr03 : "209 " #tap - right hand

sdrd3 : "209 " #tap - left hand

sdr04 : "G85 " #bore #1 - no dwell

sdrd4 : "G85 " #bore #1 - with dwell

sdr05 : "202 " #bore #2 - no dwell

sdrd5 : "202 " #bore #2 - with dwell

sdr06 : "208 Boorfrezen " #misc #1 - no dwell

sdrd6 : "208 Boorfrezen " #misc #1 - with dwell

sdr07 : "262 " #misc #2 - right hand

sdrd7 : "262 " #misc #2 - left hand

sdr08 : "241 " #drill cycle 9

sdrd8 : "241 " #drill cycle 9

sdrillcyc : "" #Target string

 

fstrsel sdr00 drlgsel sdrillcyc 18 -1

# --------------------------------------------------------------------------

 

The cycle description are OK, but the cycle time for the '241 - Gun Drill' give me '0.0'.

 

Any ideas where i can get the right cycle time??

[cadman2112]

Adding them in for selection can be done at the bottom of the post in the control def section

 

 

With the cycle time, you can't with that kind of addition,

 

You've created what is essentially a point path with parameters you set in place.

 

there is nothing for Mastercam to calculate for cycle time

[Henk]

_{"there is nothing for Mastercam to calculate for cycle time"}

 

_{It is an drill cycle, in backplot there is a path length and cycle time}

[Henk]

Bump:

 

 

That gundrill cycle is in the "drill_cycle_9" position, maybe that's the problem ???

[Colin Gilchrist]

Henk,

 

The Custom Drill cycles do not process like normal Drill Cycles in MP. You are not going to get any cycle time calculation for the custom cycles, unless you write your own logic in the .SET file to calculate the feed/rapid motion distances and then call the time calculation post blocks.

 

When the .SET file begins processing, the first post block to be called is 'pprep$' in this post block, you'll find the following code:

  usecandrill$ = no$   #Use canned cycle for drill
  usecanpeck$  = no$   #Use canned cycle for Peck
  usecanchip$  = no$   #Use canned cycle for Chip Break
  usecantap$   = no$   #Use canned cycle for Tap
  usecanbore1$ = no$   #Use canned cycle for Bore1
  usecanbore2$ = no$   #Use canned cycle for Bore2
  usecanmisc1$ = no$   #Use canned cycle for Misc1
  usecanmisc2$ = no$   #Use canned cycle for Misc2

 

You can see that in 'pprep$' we are disabling the canned cycle output. This causes MP to calculate the motion as 'G0/G1' motion. This motion is buffered internally by MP, and when the 'NCI gcode$ 81 line is encountered', the buffer is recalled and each motion block is output. Because the motion is broken into 'G0/G1' moves, each buffered piece of motion calls either 'prapid$' or 'plin$', which in turn calls 'ptime' to calculate the time.

 

That is the reason you aren't getting any cycle time, because MP cannot break up and buffer the motion. The reason is that the normal drill cycles use common variables, and the processing is well defined. Custom Drill Cycles are just that; custom. The post writer is responsible for doing all the calculations for motion.

 

In your case, adding code to properly calculate this motion and time is certainly possible, but it is also a fair amount of work.

 

To do it properly, you'll need to add 'pdrlcst$' and 'pdrlcst_2$' post blocks, and add the code in there to calculate the rapid and feed distances. Once you've calculated the distances, you can call 'ptime' and have the time output calculated.

 

Hope that helps,

 

Colin

[Henk]

Hi Colin,

 

Thanks for the info.

I'm not a postguy, but i will try to get it running.

[Roy Zomer]

If we take cycl 208 (milling a hole) or cycl 262 (milling a thread) and we choose to do these operations with a drilling cycl, Mastercam will not calculate the distance the mill is traveling. Only a straight line downwards and the feed rate it's programmed.

If we choose to program a circle mill toolpath (helix bore) (thread mill) would be the easiest way to get the actual time.