Verify Time way off.

[Thoob]

Hi everyone. I have a question about when I go to back plot to check a cycle time, its way off to what my machine is cutting. I am cutting 4 holes in a big plate. I am drilling 2.5" first, then using a 2" high feed mill to rough to 4.5 then a finish 2" 90 degree insert cutter to finish to 4.531 +- .0005. Now the thing is Mastercam shows my cycle time as 44 min, 57 seconds. The thing is my cycle is taking 72 mins total. 27 mins difference. This is a lot and could really hurt me when I do a quote. Is there anything you guys might know of as to why its calculating that fast? My rapid time is 5 secs. The rest is feed time.

[pantherprogrammer]

One thing that would help is to check the setting in your control definition. Make sure the rapid traverse rates are set correctly, tool change time, etc.

[Thoob]

Ya I have my rapid speed set properly but I don't see an option to adjust a tool change time. I am in my general machine parameters. However I don't think the 2 tool changes would affect a 27 min difference though would it? lol. I am not in control def though. Where in control def are settings for rapid speed?

[John Morris]

Off the top of my head:

 

-Make sure to eliminate the obvious first, make sure machines overrides are all at 100%.

 

-Open the program in the Cimco editor and go through the NC functions-Toolpath statistics and see what that gives you.

[Scott Lundin Shopware Inc.]

One thing that will cause incorrect cycle time calculation is the fact that Mastercam does not count additional time for peck drilling.

[gcode]

This is a reported bug.

I know its true for contour ramp..

I haven't worked it out for cicle mill/helix

From my bug report August 2009 logged as

CNC 00060183 (Version was X4 )

 

quote:

---

The toolpath is a Ø10" circle

ramping 1" deep at a .100 pitch

or 10 passes at a feedrate of 10 ipm

 

10" x Pi X 10 passes = 314"

314" / 10 ipm = 31.4 minutes

 

If you check backplot /info,

both cycle time and path length

are off by a factor of 2.

---

 

[ 07-23-2010, 08:17 AM: Message edited by: gcode ]

[Thoob]

Ahhh. That would be it then. I am using a contour ramp for my finish. My drill is not pecking though. Its a 2.5" Sandvik 880 drill. Ok thanks alot gcode. appreciate it.

[pantherprogrammer]

Thoob,

I did mean machine def. Sorry to send you on a wild goose chase.

[Verndog]

Thanks Gcode...I've been looking for the cause of this forever! I know canned cycles can be way off depending on peck amount and retract inc. distance params set on CNC machine also.

 

To expand on that same test using X3 here is what I found.

 

Using ramp depth of .1 to equal 10 passes.

Linearize helix on 31.24 m (correct)

Linearize helix off 15.42 m (wrong 1/2 the time)

 

Same error occurs using ramp angle also.

 

Bottom line, if you want accurate time turn linearize helix on with arc (helical) ramping (and change back to post). I'd imagine this will carry over into many paths that do helical entry, possibly even threadmilling.

[gcode]

you want a really kinky bug I just found??

draw 2 identical circles

same size, color, level etc..

chain 1 circle

do a contour ramp with comp type = off

 

the toolpath zigs back and forth cw then ccw

posted code is

g2

g3

g2

g3

etc..

 

delete the duplicate and regen.. all is good again..

waiting for a bug number on this one..