surface finish choppy

[tpsimer]

I am using Master cam to program profiles on a Fanuc controller. I have a Y axis on the left spindle but not on the right. I cannot cut the square profile on the outside of the part on the right side though because it is off center of the bore. I am boring, face drilling, cross drilling and pocketing on the left side and handing off to the right to locate on the bore. The outside profile is rectangular with a couple of radii on it and is off center. MCam programs using x and c in steps all the way around and leaves the surface finish choppy. Will using the 12.1 polar interpolation help with the surface finish. I sure know it will help with the length of the program. I don't have enough room in the controll to even deburr the outside right now.
thanks
tony

[dcoupar]

Originally Posted by tpsimer I am using Master cam to program profiles on a Fanuc controller. I have a Y axis on the left spindle but not on the right. I cannot cut the square profile on the outside of the part on the right side though because it is off center of the bore. I am boring, face drilling, cross drilling and pocketing on the left side and handing off to the right to locate on the bore. The outside profile is rectangular with a couple of radii on it and is off center. MCam programs using x and c in steps all the way around and leaves the surface finish choppy. Will using the 12.1 polar interpolation help with the surface finish. I sure know it will help with the length of the program. I don't have enough room in the controll to even deburr the outside right now. thanks tony

I just ran a comparison between X-C and G12.1 interpolation on a Doosan TT1800SY. The G12.1 finish was definitely superior.

[angelw]

Hi Tony,
Dave's comparison confirms what is a most logical conclusion. When using Polar Coordinate Interpolation, the control system calculates a trajectory the same as it does for any other synchronized move. Accordingly, there will only be one acceleration/deceleration phase per move command in G12.1 as opposed to the many when the profile is generated via many small moves. See the Thread in this forum titled "C-Axis Post help" to see a comparison of program size between Polar Interpolation, and the profile generated using small X-C moves.

Regards,

Bill

[tpsimer]

Originally Posted by angelw Hi Tony, Dave's comparison confirms what is a most logical conclusion. When using Polar Coordinate Interpolation, the control system calculates a trajectory the same as it does for any other synchronized move. Accordingly, there will only be one acceleration/deceleration phase per move command in G12.1 as opposed to the many when the profile is generated via many small moves. See the Thread in this forum titled "C-Axis Post help" to see a comparison of program size between Polar Interpolation, and the profile generated using small X-C moves. Regards, Bill

I read that before posting here. I even copied the sample post to generate my program from. The post just didn't talk about surface finish. Generally I don't care about the size of the program except when it won't fit in the machine controller. I only have this problem at work. At home I built a cnc router and run programs from a couple hundred lines to 400,000 lines and more doing artwork. Hopefully the boss will see the advantages of doing the milling operations on the twin spindle lathe vs lathe ops followed by two to three mill ops. Where I have the most trouble fitting programs is when I have to do engraving of part #'s and such. This is where I am trying to get him to either get more memory or a small laptop for dnc.
Thanks,
Tony

[ALEXCOMO]

Ok is for the precision , Fanuc is famous for chopping.... but it have reason, for the precision a cnc contro may DO a deceleration aT the end of a g code block, istead if you are doing a 3d parT you need to start a g08 or g5 for smoother the movement.
But we are talchink of lathe then on 0ITC usually the producer put on Mcode to actiivate g62 G64 is not a solution but he can smothing .

CHECK PLC SIGNAL G053 BIT6 TO FIND RIGHT M CODE