Ridiculously long run times

[Francis Farmer]

When your speeds and feeds all seem to be in line, and you are using a particular tool to cut one contour, and the times are great; what do you look for when the same tool cutting a circular tool path (counterbore, no finish or roughing passes) takes a year (5 hrs.). All of my speeds and feeds are the same. Is it something in my tool def.? What sorts of things do you guys look at?

 

Thanks alot,

-Francis

[Scott Bond]

Hi

 

Are you ramping at,, say 1 degree?

[Brendan P]

Sounds to me like you may have created the tool

yourself instead of "picking" one out of the library.

The reason I say this is that every time I do this,I forget to assign a feed to the tool in

set up, and it usually "defaults" to .01 IPM

which is extremly slow!

 

Just a wild guess.

[Tony]

I circle mill C'bores too.

(Mostly because people try to hand sharpen the c'bore tools and Ruin them)

Here are some "Off the top of my head" #'s

The through hole is already there from a drill operation,So I circle mill from center

(I use my half worn out Solid carbide)

Z-.010 a pass @ 40 ipm 2200 rpm with flood

Bigger bores I can fit an insert cutter in there

Z-.020 and faster feeds/speeds

You can use h.s.s hog mills and take the

whole thing at once,

But only at 2.0 ipm and 200/400rpm w/Flood.

 

[ 02-06-2003, 11:07 PM: Message edited by: Tony ]

[chris m]

Does the machining actually take 5 hours? Who would watch a machine run for 5 hours milling a counterbore?!?!? Unless the c'bore is about 6 feet in diameter and 3 feet deep I'd say that's a little excessive! Hopefully this is only a MC generated time and a guy didn't come in off the floor saying "I'm going home, the second shift guy will watch the next hole."

 

But seriously, one thing it might be is a "per-rev" feedrate entered with IPM mode selected, like:

 

G94 G03 X?.??? R?.??? F.016

 

I've had this happen a couple of times; .016" IPM is REALLY slow

 

C

[Matthew]

If you look under toolpaths/job setup in the "feed calculation" box there is a switch "adjust feed on arc move". Make sure it is unchecked or has a higher value than the default ".01".

[Francis Farmer]

What I did was draw this part as a solid model in Autocad, then import it into mastercam. Could the method I used to draw the model have any bearing on how it is chained, and then posted? The machine doesn't run as long as I'm saying, the length of run time comes from the fact that on this particular contour in the g-code about every ten or so lines it is throwing out a zero feed value. When I go to load the program into my machine it throws up errors, and wont run until I change the zero feed values in the code. Nothing I have ever drawn using mastercam has given me this trouble. Should I just redraw in Mastercam?

 

Thanks for your responses thus far.

-Francis

[Francis Farmer]

Just so you know, I went through all the feeds and speeds (everything seemed Kosher), and I didn't find anything in the contour set-up box to mitigate radius feed.

[Tony]

I would call and then email the mc file and a copy of your post To your reseller.

My reseller would have it solved and back to me

the next day.

Tony

[Francis Farmer]

Matthew,

You were referring to the minimum radius feed in the job set up box. It was checked, and it was at .01!!!! You're a Superstar!!! I adjusted this value, and everything fell in line. Thank you so much, I scratched my head over this all afternoon.

Francis

[Matthew]

I was there once before scratching my head over that one!

 

Glad I could help.