Intercon help request

[lavrgs]

I want to make a circular ring (pocket) with an ID of 1" and cut a groove 0.27 in. wide. I used the ladder function and get the 1 inch circle but the groove is only the cutter width (0.25) Do I need two operations? Another ladder cutting the outer diameter?
The other issue is that there is a lead in (?) shown in the picture

[cncsnw]

The Frame cycle just cuts once around. If you want to cut more than the cutter width, you need to insert two Frame cycles.

Use the "Entrance Type" selection to tell Intercon whether you want an arc lead-in and lead-out, or whether you want to just plunge straight down at the start, and pull straight up at the end.

[lavrgs]

AHHH yes plunge strait! THX If I want the inner circle to be 1.00 inches OD using conventional cutting do I need to deal with cutter compensation? I want the outer circle to be 1.54 ID also conventional cutting. I'm guessing I need to switch cutter comp in between

[cnc_smith]

The framing cycles look at the cutter size and makes the adjustments. There is no user cutter comp involved. If you have to adjust the size of the cutter make sure you re-post the program from Intercon.

[cncsnw]

Depending on the tolerance and finish requirement, you might want three Frame cycles for that.

I would probably start with one in the "middle": e.g. an "Outside" Frame around a diameter of 1.02". Then you could finish the inner wall with an Outside Frame and a diameter of 1.00"; then finish the outer wall with an Inside frame inside a diameter of 1.54".

With that sequence, you are basically roughing most of the material out before the dimensions matter; then doing light finish passes around both your final walls.

[lavrgs]

Depending on the tolerance and finish requirement, you might want three Frame cycles for that.

I would probably start with one in the "middle": e.g. an "Outside" Frame around a diameter of 1.02". Then you could finish the inner wall with an Outside Frame and a diameter of 1.00"; then finish the outer wall with an Inside frame inside a diameter of 1.54".

With that sequence, you are basically roughing most of the material out before the dimensions matter; then doing light finish passes around both your final walls.

That sounds perfect Thanks!

Bill

[lavrgs]

I have one more question. I programmed the part using Intercon. I have my tools measured and in the tool table. I set the Z to zero at the top of the material but it seems that after I run the part I lose the original Z zero height and would have to reset it to run again...After it finishes What it thinks is zero is 2.024 above the part. What is resetting the height? do I need a move at the end of the program to go to z.25?

[cncsnw]

Look at the "T" and "H" numbers in the status window, in the top right corner of the screen.

The "H" number is the active tool height offset number. While the program is running, it is usually the same as the tool number (assuming that you followed typical programming and setup practices).

At the end of the program, Intercon usually posts both G49 and H0, either of which would effectively cancel tool length compensation.

What is the value of your tool height offset for the tool you are using in that program?

[lavrgs]

Look at the "T" and "H" numbers in the status window, in the top right corner of the screen.

The "H" number is the active tool height offset number. While the program is running, it is usually the same as the tool number (assuming that you followed typical programming and setup practices). I'm new to using tool offsets

At the end of the program, Intercon usually posts both G49 and H0, either of which would effectively cancel tool length compensation.

What is the value of your tool height offset for the tool you are using in that program? -2.0256

If I removed G49 and changed the H value to 2.0256 (should it be minus?) and saved the program with a new name I should be able to callit up and repeat .
When setting tool height do I need to take the tool setter height into account? I use a master tool and offset from there.

[tblough]

The H patameter takes an offset integer value, not the actual offset amount. If you want the control to retain the last tool and height offset at the end of the program, just delete the line containing G49 Hnn.

When setting tool heights using a tool setter, you are just recording the DIFFERENCE in heights vs your master tool. As long as you set your part height using the same master tool, you should be fine.