Mastercam Reamming

[Tedarencn]

In Mastercam there is not reamming function,right? All guys use drill operation to replace reamming?

[uncle_dolan]

Yeah I just use a standard Drill Cycle, no peck

[mkd]

often i will use a g86 bore cycle. prevents squealing/chatter on the retract and the fast spiral marks from spinning@rapid.

can be cure for randomly going oversize due to random squeal.

[NOTW Programmer]

I also use G85 bore in/bore out, Thats pretty much what you want on a tight tolerance hole, I've used G81 when I got open tolerance.

[LancoUSA]

We use G86 bore stop retract for the same reason MKD stated. We had problems with holes being over size. Have had no troubles since

[Guest]

I think what you're looking for is when creating a drilling operation, on the cut parameters branch, there is a "cycle" pulldown menu, using the pull down you can select drill drill cycles

 

G81

G82

G83

G84

G85

G86

 

and many will also support G87 & G88

 

But all cycles are created as "drill" cycles the user then selects the specific "drilling" style cycle

 

[drafting3]

i always ream by using a drill cycle, then selecting a reamer tool. mastercam defaults to g85 bore cycle (feed in/feed out) when selecting a reamer tool.

 

i've never had a problem with off-sized holes using this method.

 

 

I've never used g86. what benefit does this offer? or perhaps, what application does it have? (I always thought stopping the spindle and G0-ing out was a no-no.)

[Rstewart]

(I always thought stopping the spindle and G0-ing out was a no-no.)

 

Why is That??

[gms1]

To me it's because you are dragging cutting flutes back through the hole which would create vertical lines in the hole. I've always been a g85 fan.

[htm01]

always used stop/rapid for undersize and feed out for oversize

[drafting3]

Why is That??

 

To me it's because you are dragging cutting flutes back through the hole which would create vertical lines in the hole. I've always been a g85 fan.

 

^that's why. maybe it's not a big deal?

 

always used stop/rapid for undersize and feed out for oversize

 

does that work? seems like the hole would already be on size after feeding down, so feeding back up shouldn't matter?

 

By that logic, if you feed too slowly you will oversize your hole?

[mkd]

drafting3,

try it you'll like it.

[Guest]

(I always thought stopping the spindle and G0-ing out was a no-no.)

 

And that begs the question where did you get THAT idea?

 

When reaming and you rapid out of a hole you "can" occasionally get swirl marks as the tool rapids out. Does the cycle work, sure it works and if your reamer has .0000 runout you will rapid out perfectly fine

 

With a G86, yes it feeds down, stops the spindle, rapids out, restarts the spindle, as it stops, when it rapids you can "only" get a straight line up. From a finish standpoint, it has "visually" always been better than a swirl, I have had parts rejected that met size but not finish because of the swirl

 

G85 feed in/feed out, yes, that can help sometimes on tight tolerances where he ream size is near the bottom of the tolerance, the feed up motion "can" help control size.

 

The noobies ask questions, that's fine, we ALL had those questions, those us us with many years of experience, we don't do things just becasue, we do them because we have proven time and time again, they work

[htm01]

^that's why. maybe it's not a big deal?

 

 

 

does that work? seems like the hole would already be on size after feeding down, so feeding back up shouldn't matter?

 

By that logic, if you feed too slowly you will oversize your hole?

thats the way i learned in highschool tool&die shop

[drafting3]

And that begs the question where did you get THAT idea?

 

The veteran toolmakers here at the shop say feed in/feed out. Some of what they say I follow like gospel, but I'm always trying to figure out if it's tradition, opinion, fact, or preference.

 

I'm still learning the infinite depths of machining, and I'm always cautious about picking up bad habits from misinformation that might haunt me later.

(For example, I've been shown three different ways, by three different toolmakers, how to use the cut-off wheel to cut ejector pins to size. I'm still trying to figure out which method is "the best". I've narrowed it down to the top two)

 

I only care about fact. If it's not right, it's wrong... with very little room for a gray area.

 

When reaming and you rapid out of a hole you "can" occasionally get swirl marks as the tool rapids out. Does the cycle work, sure it works and if your reamer has .0000 runout you will rapid out perfectly fine

 

With a G86, yes it feeds down, stops the spindle, rapids out, restarts the spindle, as it stops, when it rapids you can "only" get a straight line up. From a finish standpoint, it has "visually" always been better than a swirl, I have had parts rejected that met size but not finish because of the swirl

 

 

Would you still stop and rapid out using a spiral flute reamer? Would that flute geometry magnify these (possible) vertical retract marks?

 

 

G85 feed in/feed out, yes, that can help sometimes on tight tolerances where he ream size is near the bottom of the tolerance, the feed up motion "can" help control size.

 

Wait... I thought everyone else ways saying they used G86 because G85 sometimes resulted is a looser tolerance? I'm misreading, or confused, or both...

 

 

The noobies ask questions, that's fine, we ALL had those questions, those us us with many years of experience, we don't do things just becasue, we do them because we have proven time and time again, they work

 

I am one of those noobies, which is why I'm trying to learn the benefits of each cycle. In my limited experience, there are always multiple ways to complete a specific task, but one method will always stand out as the "best" way to complete said specific task. My goal is to learn which method is the best in which situation.

 

This is what it sounds like to me so far:

 

G81 - Fastest, Poorest surface finish

G85 - Slowest, Best surface finish (sometimes oversizes?)

G86 - Fast, with good surface finish

[Allan]

When reaming a hole, I simply use a G81 simple drill cycle.

When i want a press fit hole, I get an undersize reamer.

Never had problems with surface finish since the hole dia. was always small < .500".

I can imagine that with a large hole diameter you may want to stop and rapid out or feed out with spindle running.

However, I would most likely look for another way to finish the hole.

I always concidered the G85/G86 cycles to be used with boring heads.

 

 

Allan

[gcode]

If you have good tool holders, straight reamers and minimal runout, there should be no reason

to use G85 or G86 for reaming

[mkd]

^^^been a while since you oversaw an aluminum production line, eh?^^^

[gcode]

^^^been a while since you oversaw an aluminum production line, eh?^^^

 

what's aluminum ????

around here 2 pieces is production

[krl1t0z]

pls help me

http://www.emastercam.com/board/index.php?showtopic=76644

[Guyinthedesert]

When I saw the title of this thread, I just thought he'd gotten his maintenance bill.

[Honeywell Joe]

G81, 85, or 86...They all work. Pick what gives you the result you want and then be consistent.

It's the size of the reamer, not the cycle type that gives you the desired hole size.