Favorite Ream Cycle?

[Kelly Burns]

I keep seeing a bore in/feed out coming up as defaults in several programs. I was wondering what the preffered method of reaming was for most people. I have always just G81'ed in and out of the hole using 35sfm and .0025 per tooth for most general materials.

 

Opinions please.

[crazy^millman]

Well I think it also depnds on other factros. How is the reamer being held? How true is the reamer running? How long is the reamer and is the hole thur or blind? Is it a carbide reamer, carbide tipped, or highspeed reamer? Is it on a lathe or is it in milling center? I have have most times done the G81 method, but seen in some 300m when it was giving some carbide tipped reamers a fit. Whne we changed it to a G85 which was cool on this machine where it did a double feed rate out. A little more time but went from 40 to 60 holes per reamer to over 400 holes and still looked good. Cycle time was more, but it did last and hold size with no problem.

 

HTH

[Guest]

I use G86 most of the time, I'll use a G85 for a tight toleranced hole when I am using a boring head.

 

I don't like the rapis out of the hole when reaming while the reamer is still spinning.

[chris m]

feed in feed out, sometimes double or triple feed on the way out, but no rapid for this kid

[Kelly Burns]

Thanks guys.

[Mcam Nut]

g85 for both boring and reaming here

[Cuda84]

Ream G81, if I use G85 the people running the machines have a fit.

[Guest CNC Apps Guy 1]

I'm a feed in/out guy. I don't like marks on my reamed holes walls. I want good predictable results so I do it the same every time. Coosts me a bit in cycle time but well worth it IMHO.

[Tim Johnson]

I feed out at 3x feedrate.

[titanium neck]

My favorite reaming cycle is to pull the guy aside, speak with a low calm voice outlining the mission of the company, verify through questions that he wants to work here and support the company mission, explain to him that when the company makes money, he makes money. Upon receiving an answer in the affirmative, I then raise my voice several octaves and exponetially in decibels and ask why the #%*#&^%@!!! did it take him 2 hours to drill and tap 2 holes and manage to get them both wrong.

 

Oh, I just read some of the other responses. Um never mind.

[Mcam Nut]

lmao, not that kind of ream titanium

[jeff]

I use G81 without any problems at all.

And I go by the ME Consultant for my reamer speed and feeds.

[Kelly Burns]

quote:

---

I feed out at 3x feedrate.

---

How is this being set up out of MCam?

[mcpgmr]

G81 has always worked well enough for me. As long as the reamer is being held properly I've never had a problem with this cycle. The problem I have is the guy running the machine thinks the feed is to fast and he turns the over ride back to 50% and blows the hole over size.

[Tim Johnson]

quote:

---

quote:

--------------------------------------------------------------------------------

I feed out at 3x feedrate.

 

--------------------------------------------------------------------------------

 

How is this being set up out of MCam?

---

I'll post what I use during lunch.

[Brad MacKinnon]

I use feed in/feed out. But a teacher once told me the if you are reaming to feed in, stop spindle and rapid out. To save the life of your tool.

But Like James said "I don't like marks on my reamed holes walls" this I agree on also. Dose this seem logical ? or is just a matter of weather you want marks on the walls or a reamer that will last you?

 

Ive used both cycles before and noticed minimal to no marks when stopping the spindle and raipding out.

 

 

Im glad this came up, Ive wondered about this for a while now.

[jeff]

I personally haven't noticed a difference in size between the G81 and feed in/out.

So I use G81 for cycle time reasons.

HTH

[Jack Neelands™]

feed in /feed out for me.....

[Tim Johnson]

Here's my ream cycle. Actually the retract feed is 4x feed;

 

First initialize the variable reamfeed;

 

code:

---

reamfeed   : 0     # reamer retract federate

---

The custom drill cycle in pdrlcst$;

code:

---

      if drillcyc$ = 11, # reaming cycle

[

savdrl_gcode = gcode$

reamfeed = feed*4

pdrlcommonb

pbld, n$, pdrlxy, e$

pbld, n$, *sg01, *depth$, *feed, e$

if dwell$ <> 0, pbld, n$, sg04, *dwell$, e$

pbld, n$, sgfeed, *refht$, *reamfeed, e$

pcom_movea

]

---

The custom drill cycle in pdrlcst_2$;

code:

---

      if drillcyc$ = 11, # reaming cycle

[

pdrlcst$

]

---

The text for the reaming cycle (at the end of the post)

code:

---

[drill cycle 12]

1. "Reaming cycle"

7. ""

8. ""

9. ""

10. ""

11. ""

---

Depending on how your control def is set up you may need to put the text info in Control Def/Text/Mill Drill Cycles

 

Also the cycle is drillcyc$ 11 but the text will show as drill cycle 12

 

This post is for MCX MR2. I don't have X2 loaded up yet, hopefully I'll get the disk soon. I don't know if there are any changes in this section.

 

 

HTH

[Kelly Burns]

Thanks, Ill play around with it when Ive got some free time.

[Bpin]

feed in stop spindle rapid out for straight flute

 

feed in feed out for spiral flute

 

[heavychevy2155]

I use different cycles to size the hole, bore in/out to loosen the hole if the reamer has some wear, bore in stop spindle rapid out to tighten up the hole if its oversize. I buy reamers +.0005 and -.0005 if I have tight tolearnces to hold, and test cut some holes to get some numbers to work with.