Driven Toolpath

[IDDQD]

I recently bought a Prototrak knee mill with full 3 axis capability. I also have Mastercam X. I am doing a new part for a friend and am having trouble generating a toolpath. I'm trying to use a lollipop bit to create a circular "pedestal". The pedestal exist on the right plane and I am machining from the top plane down. This seems fairly easy but I cannot get the bit to plunge down and around in the circular motion. I have not used sketches before; only surfaces to generate the toolpaths. And I'm starting to get a headache Anyone willing to help?

[Matt Berube]

Is this what you're trying to do ?

This is mostly a guess...

I whipped this up with a DEMO version. I'll do it over tomorrow and save the .mcx if this is what you want.

There is going to be a problem, though...

With the fillet being .0625 and the height of the boss being .0625 as well, this would be impossible to machine since your lollipop "shank" dia would have to be ZERO (or less )

Or do I have it all wrong ?

Click the picture for a better view. The tool shown is a .25 dia lollipop with a .125 shank.

[IDDQD]

That's exactly what im looking to do. The size of the fillet is negligible as the pedestal is for a bearing race, and there are no other clearance issues. That looks like it was incredibly easy to do. Thank you.

[Matt Berube]

This is what I did...

Some of this procedure could be considered a bit of a hack job but I believe the strategy will work.

1. Open your .igs in Mastercam X MR2
2. CREATE>>CURVE>>CREATE CURVE ONE EDGE, Select the large flat face and drag to the edge near the base of the fillet.
3. EDIT>>SIMPLIFY, and select the "curve" you created. It initially generated a spline and we will get better results if we "simplify" it to an arc.
4. XFORM>>TRANSLATE the arc X.125 (radius of the tool)
5. Load a Machine Definition, TOOLPATHS>>CONTOUR TOOLPATH, Chain the curve you created.
6. Select the tool, enter "planes" within the toolpath and set the "comp/construction plane" to "right side"(that is the most important step), set tip comp center, set compensation type off, set XY stock to leave to .045 (visual estimate adjust as necessary)

Unless I've forgotten something I think that should just about do it...

This still probably isn't a realistic operation if you consider that I reduced the "shank" of the .25 dia lollipop mill down to .12 dia. That wouldn't exactly be a very rigid tool...

But anyway, this should be a good example for you.

I am e-mailing you the .mcx file momentarily.

To actually cut this feature with an "off the shelf" tool, I would probably try something like Harvey Part #22932 as seen here :

http://www.harveytool.com/products/p...ting+End+Mills

[IDDQD]

Ok, I got it to work but had to do a few things different. My file isn't an IGES so I was able to just sketch an arc. Also my comp/construction plane had to be set to Front. Other than that there were no problems. I do have a tool already that is very similar to the one you posted, it should work. I'm ordering one from harveytool but its going to take a week or so to get it I guess. The actual material is aluminum so the cutter shouldn't have a problem with strength. Thanks again.

-Chris