G71 roughing feeding too fast

C

cuttergrinder

Hot Rolled

Joined

Mar 16, 2007

Location

Salem,Ohio

• Aug 6, 2020

• #1

I am trying to rough machine this shaft using G71 roughing on an oi-tc fanuc control. it roughs fine except the last roughing pass feeds real fast on the 1st step of the shaft. it feeds about .050 per rev. when it steps up to the second size it feeds normal. it also wants to feed fast on the G70 finish cycle.

 

1

13engines

Stainless

Joined

Jun 30, 2015

Location

Saint Paul, MN

• Aug 6, 2020

• #2

How can anyone possibly help you if you don't post your exact code being used? Maybe even include an outline of the part.

 

C

cuttergrinder

Hot Rolled

Joined

Mar 16, 2007

Location

Salem,Ohio

• Aug 6, 2020

• #3

here is the program

 

Attachments

• 
  20200805_133828.jpg

  97.2 KB · Views: 145

C

cuttergrinder

Hot Rolled

Joined

Mar 16, 2007

Location

Salem,Ohio

• Aug 6, 2020

• #4

that's the first part of the program. I guess I didn't take a picture of the rest of the program. I'm at home now. I'll have to get the rest tomorrow

 

C

cuttergrinder

Hot Rolled

Joined

Mar 16, 2007

Location

Salem,Ohio

• Aug 6, 2020

• #5

I was working on it while you were typing.

 

K

kctallguy

Aluminum

Joined

Nov 10, 2012

Location

usa

• Aug 7, 2020

• #6

Check to make sure you have a G01 in the canned cycle starting at the appropriate feed line between your N100 and N110 numbers. If it's not there it will rapid across the last step of the cycle.

Sent from my Moto G (5) Plus using Tapatalk

 

C

cuttergrinder

Hot Rolled

Joined

Mar 16, 2007

Location

Salem,Ohio

• Aug 7, 2020

• #7

that was the problem. no G01. I'm surprised that it didn't just try to cut the whole thing in rapid rather than just the last pass.

 

G

guest

Guest

• Aug 7, 2020

• #8

cuttergrinder said:

that was the problem. no G01. I'm surprised that it didn't just try to cut the whole thing in rapid rather than just the last pass.

Click to expand...

cuttergrinder said:

...it also wants to feed fast on the G70 finish cycle.

Click to expand...

If you don't want the finish pass at .014" IPR, put the feedrate for the G70 pass on that same G01 line.

 

S

sinha

Titanium

Joined

Sep 25, 2010

Location

india

• Aug 11, 2020

• #9

cuttergrinder said:

that was the problem. no G01. I'm surprised that it didn't just try to cut the whole thing in rapid rather than just the last pass.

Click to expand...

As a rule of thumb, the profile should be defined by G01, not G00. Though it will not affect the roughing passes, the step-removal pass (as well as G70) will use G00/G01, whichever is used to define the profile.
However, the first profile-definition block (P-block)should have G00; otherwise G70 will approach the part with G01, wasting time.
Another point to note is, G71 uses the feedrate defined in its calling block. The feedrate defined between P-Q blocks is used by G70.