[svarzaru]

I am researching CAM packages for 4 axis milling. I am currently looking at FeatureCAM and for the life of me I can't figure out how to mill this object by using my 4 axis with a simultaneous 4 axis machining strategy. I would expect that this part should be easily milled from a bar mounted in the 4th axis and having the y axis move to allow the tool to reach the undercuts.

Please don't suggest other strategies, I am specifically looking on how to do 4 simultaneous axis.

[vf1kf]

I would do:

Features->Surface->Single Operation->Specialized Strategies/Four Axis Rotary

Hope that helps, let me know if that's not what you're trying to accomplish, and I'll try to be of more help.

EDIT: I'm sorry, I see now the undercuts, the above will not work. I have only the 4th axis module, which allows indexing and axis substitution, I think you would need the 5th axis option to get 4 axis to work simultaneously.

[mrprecise]

This is can be done using your 4-axis mill with a little creative CAD work.

Take your end view, as seen in your picture, and make a copy of the shape rotated in 2 or 3 degree increments, for each copy. You will have about 30 pages, showing the part rotated on the rotary axis centerline.

Now superimpose the shape of your roughing end mill in each view, leaving a clearance so you don't cut into the final shape.

Each view will have the rotary "A" angle, the Y offset which is the distance from the rotary centerline to the tool spindle centerline, and the Z offset which is the distance from the end of the tool to the rotary centerline.

Write down the A,Y,Z dimensions, and the X axis can traverse the length of the part for each rotary angle change.

One set of coordinates will be the roughing program, and the second set of coordinates are made with a ball mill for the finish program, which is tangent to the shape for each rotary angle.

Hope this helps.

[mrprecise]

Is the cut out shape a true circle?

If so, a ball mill at the center of the ball, would describe a circular path within the shape. That ball mill center position is directly related to the center of rotation of your 4th. axis.

For every 4th. axis rotary position, there is a calculable "center of ball" path/position.

You could use Excel to do the calculation for successive rotary positions, and output A*.***,Y*.***,Z*.*** for as fine rotary position steps as needed.
Then edit between each position, and add the X traverse position.

Of course, before the ball mill op, you could do 6 or 8 passes with a rougher, at different rotary positions, to clean out the bulk of stock.

[wheelieking71]

it would appear to me that you guys are suggesting ALOT of manual writing of G-code. which is very "do-able". but i dont believe thats how the OP wants to handle this. i interperet his question as "how can i program this in FeatureCAM so the software produces code that works"? and i have to say, after messing with it myself for an hour or so, that its a very good question! i am no 4th-axis wizz, but i have been messing with it ALOT in the last 4 weeks. and, with it all being fresh in my mind, i cant figure out how to get the Y-axis involved to cut that notch. and without Y, that feature is not happening in the single set-up the OP describes.

[mrprecise]

Hi wheelieking71:

Thanks for responding to my suggestion.

I understand (sort of) the OP question. However, a lot of CAD/Cam packages address the basics, and this problem is not a simple, basic operation. There is the problem of avoiding the right and left sharp edges of the pocket/hole cut-out, yet rotating A, while moving Y and Z to follow the correct path.

As the 4th axis rotates, the center of the hole being machined moves in Y and Z, and the corner/edges of the hole move closer to/or away from the cutter. The point of tangency, of a ball mill, must move in an arc, but the center of that arc is constantly changing, for every change in the rotary axis.

It is not too hard to visualize everything in sync, and sketch it on paper or talk to another machinist, but our wonderful machines only speak Gcode.

It is my opinion, as I stated above, most CAM packages do not solve two simultaneous equations, in real time, driving a cutter. I may be way off base, but this is my experience. I have used Excel to generate some difficult 4th. Axis machining code.

Perhaps this can be done in a high-end, CAM program, but I do not have unlimited funds. Some years back I did a really goofy 4 axis machine job that involved cutting an elipse wrapped around a cylinder, with an inside cut-away, like the letter C on it’s side, with the opening facing inwards. The company had the full-on Solid Works, with double screens, and all the bells and whistles. Must have been over 20K$$ in software. I was truly impressed with what kind of computer equipment they had.

All I asked for, was a TRUE centerline path, and I would do the prototype.

Well, what I got was worthless crap. After working for two weeks with their numbers, I gave up, and produced the centerline path in my Excel program. When you cut a shape with the machine, the numbers HAVE to be a “Fair curve”, or the machine jumps and jogs like crazy. I did produce the part, as per print. They didn’t have a clue. Lots of BS out there in computer land.

When you talk about writing a lot of code by hand, I am not talking about solving 500 trig equations on paper, and writing down each coordinate; just enough trig equations to solve about 5 or 6 points.

Perhaps I just like solving problems, and I really like this one!

************
Imagine the part, as shown in the graphic, with a ball cutter just tangent to the cut-out, on the right side. Now rotate the rotary axis CCW, as the ball mill simultaneously follows the cut-out until we are all the way over on the left side, and the ball mill is tangent to the other side of the cut-out.

(Path 1) The path of the center of the cut-out makes a CCW arc from about 2 oclock, moving to 10 oclock.

(Path 2) The path of the ball mill (center of ball), makes an arc CW, from about 4 oclock, moving to 8 oclock.

These two paths are moving simultaneously.

The radius of path 1 is a constant.

The radius of path 2 is a constant. (path of the ball mill ball center)

The distance from the Rotary axis center of rotation, to the ball mill center is the solution we want, for each change of the rotary axis, and the moving path of the ball mill. This distance is the foundation for finding the correct “Y” and “Z” position.

This distance is the Hypotenuse of a right triangle; a constantly changing distance, based on two variables.


The vertical distance (Z) at the start is a Known, from CAD drawing.
The horizontal distance (Y) at the start is a Known from CAD drawing.
The angle of this triangle (A) at the start is a Known from CAD drawing.
The angle from rotary center to the center of path 2 at the start is known.

For each "clock tick CCW of path1 (Rotary axis), there is a change of the center of path 2.

In Excel, horizontally across the page:

For each clock tick of path 1:
1. Solve the height, and horizontal distance of path 1 (center of path 2)
2. Increment path 2,(the ball mill path) CW, from new center.
3. Solve for location of the new ball center relative to path 2 center.
4. Solve for distance from Rotary center, to ball center (Hypotenuse)
5. Solve for horizontal distance to ball center (new Y position)
6. Solve for vertical distance to ball center ( new Z position)

I would put each particular formula in a separate column. This makes it easy to check your math.

Once you have the formulas working to produce the correct dimension, copy and paste down, with the Rotary angle incrementing the correct amount.
The increments for path 1, and path 2 must be the same number of increments. They both begin and end at the respective end of their arcs, but must be the same number of increments, although the amount of angular change will differ.

Put in a column for: "A", A value, "Y", the Y value, "Z", the Z value

Alternate rows will have the "X", and X value. The cutter traverses in X, however long the cut must be. This is the only part that you have to kludge around to insert into the Excel produced code. You can use "find and replace" in the text editor.

You can make 20 increments, or 2000. Excel can produce as many discreet steps as you want.

Copy and paste the columns you want to a text file. This is your new Gcode.

I guess there are about 5 or 6 trig equations, to get the new Y,Z.
It will take some time, and playing around. You can do two points in the CAD program, and use those to check your Excell formula.

Sometimes, to machine a part, you have to just grind it out. It really doesn't take that much time. Also, it is a good mental exercise.

As they say, thats my "2 cents"

[wheelieking71]

well, i follow that. i couldnt figure it out myself LOL. but i do see what you did there. and your "2 cents" is worth a whole lot more than you think!

[mrprecise]

Well thanks, wheelieking71. I do appreciate that.

[Kiwi]

Is the picture shown, an example of the type of work you want to machine or do you particularly require that shape?

[Excelmachine]

Could this be done by mounting your bar offset from the main central axis in x so that the center of your cut is your x axis center of rotation? Then it seems that what you want to accomplish could be done.

[mrprecise]

Hello Excelmachine:

Although I am not the OP of this thread, you idea is excellent. This is what is good about a multiple heads working on a problem.

Still a bit of a programming problem, but half the calculations from my post.
However, not so simple to get the proper centerline offset, since the circle cut-out appears to be offset in Y and Z, relative to the blank center line. Tooling and setting up the proper starting points relative to the cutter is a problem.

[Kiwi]

Have you tried with a lolly-pop shaped cutter?