mill/turn 5 axis simultaneous machining & work offset

[M Code]

Hi

This is a beginners question..
When we have mill/turn machine where the C & B are rotary axes, and we work on 5 or 4 axis simultaneous machining operation. During programming/setup do we refer the work offset to G54 for a center of the part (as simple turning operation) or there is another way to do that? like 68.2? table work offset? workpiece work offset?

What are the common ways for work offset assignment from programming/setup side for 5 or 4 axis simultaneous in mill/turn machine?

Thanks...

 

[CNC Hacker]

It would help if you said what machine and control you're working on. But generally you're going to use Tool Center Point control G43.4 to do full 5X simultaneous. G68.2 is for 3+2 work. On a mill turn usually your work offset for XY is going to be the center of the part since you're probably going to turn it as well. But it doesn't have to be, I've set up vises and fixtures in Integrexes where I was using the machine just as a 5X mill. In that case I put the work offset wherever was convenient for that operation.

 

[M Code]

It would help if you said what machine and control you're working on. But generally you're going to use Tool Center Point control G43.4 to do full 5X simultaneous. G68.2 is for 3+2 work. On a mill turn usually your work offset for XY is going to be the center of the part since you're probably going to turn it as well. But it doesn't have to be, I've set up vises and fixtures in Integrexes where I was using the machine just as a 5X mill. In that case I put the work offset wherever was convenient for that operation.

Since you mentioned Integrex let us take it an example.

In 5 axis simultaneous, I can have the work offset X,Y on the center of the round workpiece and Z on the face (as lathe), and run it with G61.1 and G43.4 but in that case what should be the parameter of F85 bit 2: (1 OR 0)? Do I need to consider any parameters?

In case of 4 axis simultaneous when B axis is fixed is it the same concept? what if i use G43P1 instead of G43.4 during 4 axis simultaneous?

Thanks

 

[CNC Hacker]

Integrexes from the factory are going to be set for workpiece mode TCP, with F85 bit 2 = 1, again because most of the time you're turning too so the work offset at the center of the part makes the most sense. Workpiece mode doesn't work for off center work offsets without using G54.4 as well. But if you set it to table coordinate mode with F85 bit 2 = 0 you can put the work offset anywhere in the machine envelope and it will track it properly. The most important thing is matching the parameter setting with the posted output from your CAM software.

I generally like to use G43.4 for 4X simultaneous as well. I've heard of people using G43 P1 for that application, but the P1 mode is really meant for turning tools. If you already have G43.4 it's easier to use.

 

[M Code]

Integrexes from the factory are going to be set for workpiece mode TCP, with F85 bit 2 = 1, again because most of the time you're turning too so the work offset at the center of the part makes the most sense. Workpiece mode doesn't work for off center work offsets without using G54.4 as well. But if you set it to table coordinate mode with F85 bit 2 = 0 you can put the work offset anywhere in the machine envelope and it will track it properly. The most important thing is matching the parameter setting with the posted output from your CAM software.

I generally like to use G43.4 for 4X simultaneous as well. I've heard of people using G43 P1 for that application, but the P1 mode is really meant for turning tools. If you already have G43.4 it's easier to use.

Thanks,
in Integrex..

1- Do you use invers time with G43.4? do you recommend to use inverse time during 5 axes simultaneous machining?
2- For 3+2 positioning do use G68.2 or G68? if I use G68 will I be able to use G02,G03 (interpolation) or G41 G42 (tool comp.) during programming?

 

[CNC Hacker]

I never use inverse time feed rate anymore. With G43.4 you can just give it one IPM feed rate and the machine will figure it out from there. It's much smoother that way.

I prefer G68.2, because if you are doing something with an off center work offset, it will track the part thru space. G68 will not do that. But most people use G68 on Integrexes just fine, because they are on center. With both of them you have the full list of things you can do with a normal 3X program available: canned cycles, cutter comp, probing, etc.