[Busted]

hi, i am totally new to this and i am trying to help a friend who is programming a cnc lathe. the machine is a puma and the control is a fanuc although not sure which series.

our problem is the machine runs the first part of the G71 roughing cycle fine with good swarf control, but the G71 cycle has a final finish profile and the depth of cut is too small to control the swarf and it wraps around the tool.

we are running at big depths of cut and high feed with roughing inserts to remove stock, and an insert with finishing geometry isnt strong enough to cope

can we increase the depth of cut for the final profile, or better still remove it completely as there is a finishing tool with finish profile chip breaker that goes in afterwards anyway

we were hoping to run the machine unmanned but the swarf gets in the way

can anyone help please

apologies for any mistakes as i am totally new to this forum and programming.

thanks very much

[Geof]

To my knowledge you cannot remove the final profile but by changin your D value you can make it the same depth of cut as all the other passes.

For instance if your start diameter is 2.200 and the finish is 1.780 you are taking off 0.42 on the diameter or 0.21 on the radius. If your D is 0.05 you take four cuts at this depth then a final pass at 0.01 depth of cut; if you change the D to 0.051 you take only four cuts all the same depth of cut.

If you have a finish allowance with a U value (I think it is U) it is necessary to take this into account in the amount taken off on the radius.

This works on Haas machines running in Fanuc mode so I think it should work for you.

[Busted]

hi Geof, thanks for the reply, i will take your answer into the shop when i next go in and see how we get on, as i said my friend is the programmer, i just look at this site when i get stuck and try an find answers, which i normally do.

your answer does make sense to me though, so i will give it a try.

thanks again

Andy

[warfreak]

id just like to add that for the finishing allowance make sure to adjust (U) and (w) for x and z respectively.

also changing the initial point that you go to before the canned cycle starts may also affect the final depth of cut



gl
:banana:

[Busted]

thanks for the reply, i dont seeem to get email notification when a reply is posted so didnt see your answer, i am back at work on the 5th so will give this a try

thanks again
A

[g-codeguy]

thanks for the reply, i dont seeem to get email notification when a reply is posted so didnt see your answer, i am back at work on the 5th so will give this a try

thanks again
A

If you aren't getting email notification of replies to a post of yours, there is a good chance that you didn't elect to get them when you registered. When you first log in look in the middle of the page about 3-4 inches down. You should see "Edit Your Profile." Once you click on this look at the options on the left. Choose "Edit Options." You can make sure it is set up to receive email notification here.

In a 2-block G71 call the U-value in the 1st block is for the depth of cut. As an example I ran an aluminum job a new guy had programmed using Mastercam. He had used the default DOC which was .1. His last pass was taking .0008 off. Since he had also used the default lead in/lead out, I modified the program on the machine. I also deleted his CSS since it was a rectangular block and could only run so fast because of vibration. Being aluminum I ran it as fast as it could go without vibration. I cut a 15 minute cycle time to 7.5. Could have cut more, but didn't have time to modify his ID work.