[newbie23]

I am pretty new to CNC Milling so bear with me. Let's say I am spotting and drilling a hole in the O.D. of a ....hockey puck (easier to describe than actual part!) When I spot the hole, the chamfer is always bigger on one axis than the other because of the roundness of the part. I really don't like that look. On a Hardinge TwinTurn, i use circular interpolation and the bar rotates back and forth to put an even chamfer on the hole, but i don't know what to do on a mill. I'm assuming that I can do it with 4 - X,Y,Z, moves. I learned that this was going to be a problem when I used an Excel Spreadsheet to make a threadmilling program and there were "J" and "I" moves in the program "still don't understand what they are but it works!!!". Can someone make a sample program for me to learn from? And possibly explain the J and I moves? I do not like to make a program and not understand what every single block means!!! Thanks In Advance!

I am using a:
Fadal VMC 88HS
5/8"-90 Degree Indexable Spot Drill

[Jake E.]

J and I moves are in relation to X and Y moves. They take the place of R. Exapmle being :

G1G41D51X.25(tool moves in compensation to .25" from starting point in the X)
G3I-.25(makes a CCW complete circle at .25 radius starting at X.25 and ending at X.25 (center at 0,0, 180deg position at -.25"))
G1G40X-.25(tool moves back to start without compensation).



Same hole cut but in the Y axis as opposed to the X
G1G41D51Y.25
G3J-.25
G1G40Y-.25

From what I understand, using I and J is also more precise.

[christinandavid]

When I spot the hole, the chamfer is always bigger on one axis than the other because of the roundness of the part. I really don't like that look.

I love that look myself, but only when using a really nice cutter. If the drawing asks for a 'true to view' chamfer and gives me the chamfer depth over component centreline in said view/section, that's what they get.

If I were compelled to follow a cylindrical surface with a ballnose cutter I would use linear increments and parametric programming to trig out the Z height at each position.

DP

[scadvice]

If I fully understand what your saying, the only way to truly produce what you’re asking for is to do XYZ 3D point to point moves following the hole edge profile. (No cutter comp) It’s kind of like looking at a round potato chip from the side.

However, you can also cheat and do it with line arc move in a XZ arc or YZ arc depending on the puck orintation.

This can be done with a end mill that has a 90 degree tip. The last time it wrote a program to do this was for a prototype part in plastic. It was done on a Haas indexer but the actual moves were done as I stated above.

There were multiple holes and I had to do a radius on them. I can post a picture as I still have a sample part but you would have to wait a week and a half as I'm out of town on vacation.

Steve

[newbie23]

J and I moves are in relation to X and Y moves. They take the place of R. Exapmle being :

G1G41D51X.25(tool moves in compensation to .25" from starting point in the X)
G3I-.25(makes a CCW complete circle at .25 radius starting at X.25 and ending at X.25 (center at 0,0, 180deg position at -.25"))
G1G40X-.25(tool moves back to start without compensation).



Same hole cut but in the Y axis as opposed to the X
G1G41D51Y.25
G3J-.25
G1G40Y-.25

From what I understand, using I and J is also more precise.

That makes sense to me. When I get time I'll do a simple program and see how the machine reacts to completely understand it. I bet it also explains why one of my previous prototypes had holes that i pocketed out and they were slightly elongated because the program was using a G3 instead of R. Thanks!!!

[newbie23]

If I fully understand what your saying, the only way to truly produce what you’re asking for is to do XYZ 3D point to point moves following the hole edge profile. (No cutter comp) It’s kind of like looking at a round potato chip from the side.

However, you can also cheat and do it with line arc move in a XZ arc or YZ arc depending on the puck orintation.

This can be done with a end mill that has a 90 degree tip. The last time it wrote a program to do this was for a prototype part in plastic. It was done on a Haas indexer but the actual moves were done as I stated above.

There were multiple holes and I had to do a radius on them. I can post a picture as I still have a sample part but you would have to wait a week and a half as I'm out of town on vacation.

Steve

Thanks Steve, You know exactly what im talking about when mentioning that potato chip of all things lol I look forward to the picture and maybe a simple program doing a move so i can understand. :cheers:

[scadvice]

Think about your puck. You have the radius that you are trying to put the chamfer on, but you are also are placing a circle at right axis to the puck with the round chamfer tool. So, in order to do so, you have to write a little arc that follows the radius of the puck at about the center of the depth of the chamfer. That arc’s radius is from the center of the puck to that center of the chamfers depth.

It’s a very short length of that arc maybe a 1/10th of a degree or so. You’re going to have to use a G18 or G19 command with a minus or plus value and a “K” value replacing the I or J depending on the axis Y or X used. R should work also, if I recall correctly.

Here is a link that will explain it in detail:

http://www.flintmachine.com/pdfs/fad...erpolation.pdf

There are a number of other sites I just happen to get this one to pop up first off the web.

Look at page 297.

I hopr this makes sense.

Steve

[masonbcaldwell4]

when using G17 (XY Plane), the I's and J's represent incremental values in either the X or Y axis (I = X, J = Y) from the center point of the radius to the end point... I tend to program in longhand, adding more codes than perhaps I need, but it keeps things clear for me should I screw up.... a sample program might look like this...

O100 (SAMPLE PROGRAM)
G0 G90 G80 G40 G49 G17 (my safeline)
E48 X0 Y0 (safe toolchange location as my fadal likes to spit out tools)
M6 T5
E3 H5 D5 Z2.
X-3. Y-2.
G41 X-2.5 Y-1.5 (CC on)
Z.1
M1
M3 M8 S2000
G1 Z-.5 F20.
Y0
G3 X0 Y0 I1.25 J0 F15. (the center of the radius is actually at X-1.25, but this value is incremental)
G1 Y-1.5 F20.
Z.1 M5 M9
E48 X0 Y0 G0
G53 Z0
M6 T5 (i have to add this at the end, otherwise the Z axis rapids to the upper stop at M2, for some reason)
M2

hope this helps some
M4