Odd lathe behavior

[bcduncan]

I am using the mplmaster Fanuc Lathe post to output to Mach3. The problem I am having is the toolp[ath for arcs. The post output I get often causes the arc to go in the wrong direction and I have to go through the Gcode converting some gcodes from G03 to G02 or changing the radius value to negative. Can anyone offer advise? Also the G73 post values are incorrect for Mach3 but I am going to try editing the Fanuc post for correct that.

 

Bob

[Scott Garrison@Weiler Engineering]

Is this a "negative" X lathe? I had to reverse the G02 & G03's for our Mori's in order for the arcs to work. You said "some arcs" that seems impossible that all the arcs wouldn't be wrong or correct. Have you considered using I's & J's instead of R's?

 

Also, using canned cycles is not advised since they do not work correctly. This has been a bone of contention with Mastercam lathe users for some time.

 

Scott

[bcduncan]

Thank you. I am realativly new to Mastercam. Do I need to rewrite the Post processor to choose I & J format. I have the4 same issue with G73 for threading. I have seen some comments suggesting to use G32 instead but I am not sure how for force that.

 

Bob

[Mr. Wizzard]

I have a Haas GT-10 and a TL-2. I had to set up the machine so that the turrets were on opposite sides (top turret, bottom turret). Give that a try.

Then, make sure your tools are set-up properly in the program and you are programming on the correct side of centerline.

It took some time to get everything set up and oriented correctly, but now I can program and post with no worries!

[Scott Garrison@Weiler Engineering]

You can change the R's to I & J's in the control def. You might need to switch the G02/G03's in the post.

 

I use G32 as well. It's just like G01 with a feedrate that is sync'd. Purely point to point programming so the operator really can't do too much. Most changes need to be done in MC.

 

Have you asked your reseller for help with this?These changes should be pretty simple for them to handle.

[bcduncan]

Is there a document which defines the parameters in the machine tool definition (preferably with pictures)? Like what the orientation is of upper or lower turret and how to select the side of the centerline for tooling?

 

Thanks,

Bob

[chris m]

To me, if the turret is behind the part, it should be defined as the upper turret, if it is in front of the part it should be defined as the lower turret. The exception to this is twin spindle machines, where one spindle may have a turret in "front" but still "think" it is the upper turret. The only reason you should have G2 and G3 switched in your post is if your X values are all negative [many Mori-Seiki machines, including mine, are like this]; otherwise you have some problem with your Mastercam file or Mastercam itself.

 

C