Need Help!- Circular Interpolation on Lathe?

[justin bowser]

I usually do very straight-forward turning with nothing fancy but I need to face off a 1.5" dia plexi rod with the end profile being concave or convex and I'm experiencing some sort of "mantal block". From reading I've done I think I need to specify plane with G18 and then use G2 or G3 to do my pacing. On a convex "facing" I would like the center of the face to b .025 "higher" than the edges. Think of my facing cut causing the end of the rod to resemble the face of a lens

Could someone provide me programming examples of how this would work, or links to some good examples?

Thanks in advance...

Justin B.

[angelw]

Originally Posted by justin bowser I usually do very straight-forward turning with nothing fancy but I need to face off a 1.5" dia plexi rod with the end profile being concave or convex and I'm experiencing some sort of "mantal block". From reading I've done I think I need to specify plane with G18 and then use G2 or G3 to do my pacing. On a convex "facing" I would like the center of the face to b .025 "higher" than the edges. Think of my facing cut causing the end of the rod to resemble the face of a lens Could someone provide me programming examples of how this would work, or links to some good examples? Thanks in advance... Justin B.

Hi Justin,
Unless your lathe has a Y axis, it should default to G18 on start up. However, most programmers worth there salt have a Safety Line at the beginning of the program to ensure that the machine control is initialized to the modes that keeps it safe and so that no alarms are raised.

I don't generally like using tool nose compensation with a Turning Centre. Its use is very necessary with a Machining Centre, to be able to adjust the size of features when using end mills and the like. However, in most cases, component size with a lathe is adjusted with the Tool Offsets and not Tool Nose Radius Offsets. Having said that, the following program snippet has used Tool Nose Radius Compensation, as I'm unaware of the tool nose radius you intend to use.

The radius of the arc that will satisfy your criteria for the convex form is 11.2624

Regards,

Bill

G00 X1.580 Z0.200
G41 G01 Z-0.028
G02 X0.000 Z0.000 I-0.790 K-11.235
G40 G01 Z0.200

[txcncman]

Here is the convex side. Don't know when I will get back to do the concave side.

[angelw]

Originally Posted by justin bowser I usually do very straight-forward turning with nothing fancy but I need to face off a 1.5" dia plexi rod with the end profile being concave or convex and I'm experiencing some sort of "mantal block". From reading I've done I think I need to specify plane with G18 and then use G2 or G3 to do my pacing. On a convex "facing" I would like the center of the face to b .025 "higher" than the edges. Think of my facing cut causing the end of the rod to resemble the face of a lens Could someone provide me programming examples of how this would work, or links to some good examples? Thanks in advance... Justin B.

Justin,
I'm a bit confused. I looked at your question prior to the PDF file being attached, and your criteria was for the face to be O.025 "higher" than the edges, the 1.5 OD I assumed. Your attached drawing shows a convex profile .0384 proud of a 1.2815 OD, and if the radius is extended to the 1.5 OD, the face of the profile is 0.05268 proud of the OD (edges). Where does the 0.025 come in?

Regards,

Bill

[justin bowser]

My original question was dimensions pulled out of thin air just for a "how-to". Since I decided a drawing might be a better indicator of what I was trying to accomplish I made a drawing with more "real world" dimensions.

My intention was not to get somebody to write a program for me but to take these dimensions and apply them to the G2/G3 statement so I could see how the I, K, and other parameters were derived.

Thanks,

Justin B.

[angelw]

Originally Posted by justin bowser My original question was dimensions pulled out of thin air just for a "how-to". Since I decided a drawing might be a better indicator of what I was trying to accomplish I made a drawing with more "real world" dimensions. My intention was not to get somebody to write a program for me but to take these dimensions and apply them to the G2/G3 statement so I could see how the I, K, and other parameters were derived. Thanks, Justin B.

Hi Justin,
Clearly, you mustn't have a CAM system, otherwise this program would be relatively simple.

Given the information from your drawing, that is, a Diameter and a Height of the face of the convex form above the edge, or OD of the part, the most difficult task is to find the centre of the arc in Z, and the radius of the arc. Once you have these, finding the I and K values is simple, as indicated in light blue in the attached picture.



When creating a lathe program, you only have to deal with Radial X values on one side of the X centre line; the other side being a mirror image. Therefore, as I see it, the easiest method of obtaining the Z centre and radius of the arc manually, is to use the Arc through 3 Points method. The three points will be 1 and 2 shown in the attached picture; easily obtained from your drawing, and the 3rd point being the corresponding negative of point 2.

Once you have the Radius and Centre of the arc, pythagoras theorem can be used to obtain the K value. The "I" value will simply be the radial value of where the cutting tool starts in X. If you don't use Tool Nose Radius(TNR) Compensation in the program, the centre location of the Tool Nose Radius is calculated, and the X, Z coordinates obtained by subtracting the TNR and twice the TNR from Z and X respectively when using a Right Hand Turning tool.

If you don't have the math for Arc Through 3 points, Post back and I'll supply.

Regards,

Bill

[justin bowser]

Hoo-Rah!! Between PMs between txcncman and Bill's posts to this thread I have been nudged (shoved kicking and clawing?) toward the light! You helped me visualize and realize where the parameters were being derived from and the bulb finally flashed on! After this, though, I had to figure out how to make EMC2 get along with what I was trying to do. This was accomplished through the forum at linuxcnc.com. I'm a happy (well, sort of) camper. :-)