Is there a formula, or can someone explain how to figure a table of cuts to produce smooth radii, convex and concave, with a particluar diameter end mill on a vertical mill using the x and y axes? Or perhaps a reference where such an explanation might be found?
Announcement
Collapse
No announcement yet.
x y Radius Cutting
Collapse
X

BWB
The "formula" would be particular to the shape that you are trying to produce. The principle, however, would be the same whatever the shape; calculate the xy position of the cutter at any point on the geometry taking into consideration the diameter of the said cutter. This procedure is applicable to lathing, milling even grinding. A programmable calculator or a spread sheet works well. Do you have a particular shape in mind?
Gene

Guy Lautard publishes a book of tables for circular sections:
http://lautard.com/ballbook.htm
He also discusses the process in one of his "Machinists Bedside Reader" series books.
franco
Comment

Originally posted by easymike29BWB
The "formula" would be particular to the shape that you are trying to produce. The principle, however, would be the same whatever the shape; calculate the xy position of the cutter at any point on the geometry taking into consideration the diameter of the said cutter. This procedure is applicable to lathing, milling even grinding. A programmable calculator or a spread sheet works well. Do you have a particular shape in mind?
Gene
The ideal would be to machine the perpendicular flats and the radius in the same flat setup on the mill table with an endmill. The radius being too large to just use an endmill of the proper diameter.
I realize the flats could be cut separately and the radiused cut done with a boring head, or likewise done with the rotary table.
I am looking for a way to do both flat straight surfaces and their connecting radius with the same cutter in a single setup.
I don't have a programmable calculator, and probably wouldn't know what to do with it if I did, so the mathematics of this might be beyond me. I should also have mentioned that my mill is strictly manual, not even DRO.
I guess my real question is can I do it this way, or should I resort to one of the alternatives which are certainly within my capabilities? Hell, I'd like to learn something new!
Comment

This is basically the same question as the one I answered this morning.
This is how a computer calculates and draws a circle (and a radius). It calculates a series of X,Y points and colors them. If you look real close as in the closeup you can see the individual pixels. All you need to do is calculate a table of X,Y points that lie on the correct radius for the fillet you are machining. You can do that using the procedure I gave in the earlier post and increment the degrees for each point to whatever precision you can stand. Perhaps one point every 10 degrees would be sufficient.
Free software for calculating bolt circles and similar: Click Here
Comment

To be complete, this may get a bit long so bear with me. The drawing shows a 90 degree corner of a part (heavy line) and a end mill cutter as seen from above. The radius of the part's corner is R and the radius of the cutter is r. Notice both are given as radaii, not diameters. Also, the origin or 0,0 point is choosen to be the center of the radius we want to cut (R). This is marked on the drawings.
Also, I normally mill with an origin at the upper left of the part. So X is to the right and Y is down or toward the front of the machine. This seems to work out for me but you may use a different system. If so, you will have to adjust accordingly.
First the outside radius case: The tool must follow a path that is the sum of the two radaii, R + r. Assume that we start from the left and are cutting horizontally across the bottom. The curved path starts at the right end of this straight cut so I choose to call the downward direction 0 degrees. The angle, going CCW from this starting position is given by a in the equations. The coordinates of this path will then be given by the following equations:
X = (R + r) sin(a)
Y = (R + r) cos(a)
X and Y are both positive as they are in the same direction as the given X and Y axies. This path continues until the desired final angle is reached. It is 90 degrees in this example but could be any angle.
For the inside radius case: The only thing that changes for the inside radius cut is you must use the difference between the radaii instead of their sum. This is plain to see in the second drawing as the two radaii go in opposite directions. So the equations become:
X = (R  r) sin(a)
Y = (R  r) cos(a)
Of course, your actual zero point when machining the part will not be at this (0,0) point. You must, therefore, add or subtract the actual coordinates of the center of the radius R to/from the results or this equation. So if your zero point is at the upper left of the part (how I do it), then you would add the X and Y coordinates of the point I have called (0,0) to the results of the equations.
For corners in other orientations, the signs of the calculated values of X and Y will change. In the coordinate system shown, a corner at the upper right would have X as a minus value and Y as a plus. In the upper left both would be negatives and in the lower left X would be minus and Y would be positive.
Of course, if you use a different coordinate system you will have to adjust accordingly.
I hope this helps.Last edited by Paul Alciatore; 02072009, 02:45 AM.Paul A.
SE Texas
Make it fit.
You can't win and there IS a penalty for trying!
Comment

Difficult.
Originally posted by BWBIs there a formula, or can someone explain how to figure a table of cuts to produce smooth radii, convex and concave, with a particluar diameter end mill on a vertical mill using the x and y axes? Or perhaps a reference where such an explanation might be found?
Comment

Here is a link to a program that will give you the info you need. You input the information such as size of radius you want, size of ball mill you are going to use, and the angular increment between steps and it will output the information.
It's setup so that you move z and y axis and then feed the cutter down the x axis. Then move z and y again and take another cut. The smaller the number you put in the angular increment part the smoother the part will be. I've not used this particular program but I've used his Ballcut program which works the same way but on the lathe to produce balls and it works real well. It takes some time to do but if you don't have the cutter and desire a certain radius it works perfect.
Go down to Rounder.Zip. Save it to you computer and there is some instructions with it also. Let us know if this works out for you.
http://www.myvirtualnetwork.com/mklotz/Jonathan P.
Comment

Another way to do this would be with a CAD program. Draw the desired part with the radius and then use the Offset command to generate a path that is outside the part's outline by the radius of the cutter you want to use. Then divide that path into small increments and read the coordinates of the end points of those increments.
One way to divide the arc would be to construct a series of radials from the center point. (Draw one and then copy in a circular array.) Extend them well beyond the arc and then use the Trim To command or whatever they call it to have them end on the arc. Keep the part of the radial that is outside of the arc. Now read the coordinates of the ends of those radials that rest on the arc.
If you use the same origin in the drawing as on your mill, this will give you the coordinates directly with no need to add or subtract anything. So there is little chance for error.
These will be your coordinates. No math needed. Well, the CAD program did it.Paul A.
SE Texas
Make it fit.
You can't win and there IS a penalty for trying!
Comment

Gentlemen, Thank you for your interest in my question and your generosity with your time and help.
There is much here for me to chew on.
One thing that is clear to me is the obligation of folks like me who are asking for help to present our questions as clearly as possible. I think I have done a less than good job of it, so bear with me for a clarification.
Imagine a square aluminum plate of a certain size, with a square hole centered within it. I want to mount that plate flat on the table of a vertical mill in such a way that I can profile its outer and inner edges leaving the radius cuts I've asked about at both the outer and inner corners. Obviously that will involve enlarging the center hole to produce those corners.
Say I need to produce .75" radius corners with a half inch diameter plain end mill. I would like to profile the straight flat edges with the end mill, and produce the radii using sequenced x y track plunge cuts on the z axis sufficiently close together to produce a pretty good finish using the one setup.
I think the explanations for how to do that are present in the answers given, I just haven't had time to digest it all. However, I did want to present my question in a clearer way.
Again, thanks to all who have responded so far.Last edited by BWB; 02072009, 01:16 PM.
Comment
Comment