Newbie- Questions about Program Point

[RC-CNC]

I am drawing a part in CAD and then drawing a .03125 (1/32) too nose radius to follow the part so see where my program points are. Where should I be drawing the program point for each insert geometry? Is it always to the front edge? What about for a diamond tool? Does that change the program point to the center/bottom of the tool?

Thanks in advance.


Swiss Style CNC Machine - Citizen L25

Where to draw virtual tool nose point for varying tool geometries?

Is Virtual Tool Nose Point the same as Tool Nose Radius Compensation?

How does G50 shift affect this? Why do we do a G50 shift?

Is VTNP only for use in TNRC?

Where is the Program Point? How is Program Point related to VTNP and TNRC?

[glenthemann]

Hmm, this is kind of hard to explain without any pictures.. Forgive me if some of my information doesnt make sense, I know the L20 control pretty well though and they are both mitsubishi..

First of all you plot your program points to the drawing, you dont worry about the tool geometry when at this stage, you just need to know the tools you are using.

Now when you set your tools, the machine will know where the theoretical tool tip is and that is the point on which that tool will make moves to. With your standard turn/face tool, when you set it you will set its diameter which tells the machine where the end face is. You will also set the core which centers the tool so you have no pip.

Now your side cutting edge is in relation to Z; With a standard turn/face tool the edge should be right on the theoretical zero point of the machine, however with other tools such as a left hand cut off the side edge of the tool is .422 with a .078 cut off from the guide bushing, or in the case of cutting off a part .500 from the guide bushing

This is where G50 shift comes in. We tell the machine to "shift" its zero point in relation to whatever hand tool we are using, or if any tool has its cutting point away from the theoretical zero. When cutting off the part you command G50 W-.5, which tells the machine to shift its zero point .5 inches in the negative direction. that way when you rapid the material out for cut off, it will move forward the extra .5 you need to cut off the part because it thinks you are actually .5 away from where the materially really is.

To better illustrate this, say you finish turning the part and youre at Z2.5. If you called the cut off tool in and told it to cut off at Z2.5 youd lose .5 of your part. You would first call the G50 W-.5 which makes the machine THINK the face of the material is only 2 inches from its 'theoretical zero', so when your cut off comes in and you tell it to cut off at 2.5 inches the material moves out that extra .5 you need because it thinks its only at 2.

There is also G50 zero setting which is done at the beginning of the program before you make any movements so the machine knows where it is once again. Your regular right hand cut off tool is at that theoretical zero point so you would think you say G50Z0 which tells it that is the zero point, but infact you have to leave a bit of material to face off right? If you want to face off say .005 you would say G50Z-.005 so the machine once again thinks the end of your material is .005 away the zero point so it adjust for it and leaves you .005 to face off so your part program points remain in relation to zero.

Tool radius compensation is need if you are cutting angles, contours, etc, with a tool with a radius, because the actual cutting point is not the virtual one. with toolnose radius compensation you tell the machine what type of tool you are using by the direction in which the cutting point is. ie if its a turning tool, a grooving tool, a backworking tool, a boring bar, etc.. I wont go into too much detail as Ive already written a book and this is standard for all machines (as far as I know) so you can find the information easy enough.


Goodluck.